Overview
Welcome to the FreeStyle Shaper, Optimizer, and Profiler User's Guide ! This guide is intended for users who need to become quickly familiar with the product. This overview provides the following information:
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FreeStyle in a Nutshell Before Reading this Guide Getting the Most Out of this Guide Accessing Sample Documents Conventions Used in this Guide

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FreeStyle in a Nutshell
FreeStyle Shaper is a powerful modeling tool used to dynamically design all types of surface elements, from the stylist's drawing to the final surface, ready for the manufacturing processes. Using this product you can generate free form 3D curves and surfaces from scratch, and dynamically deform and analyze all produced elements. Using the FreeStyle Optimizer you can create and modify curve and surface shapes based on other elements such as digitized data. Using FreeStyle Profiler, you can directly create complex surfaces based on profiles and sets of curves in one step, without having to deform them in a second step. The FreeStyle Shaper, Optimizer & Profiler User's Guide has been designed as an aid to using the FreeStyle Shaper, FreeStyle Optimizer, and FreeStyle Profiler by themselves, but also in conjunction with other CATIA Version 5 workbenches.

Before Reading this Guide
Before reading this guide, you should be familiar with basic Version 5 concepts such as document windows, standard and view toolbars. Therefore, we recommend that you read the Infrastructure User's Guide that describes generic capabilities common to all Version 5 products. It also describes the general layout of V5 and the interoperability between workbenches. You may also like to read the following complementary product guide:
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CATIA V4 Integration User's Guide presents interfaces with standard exchange formats and most of all with CATIA V4 data.

Getting the Most Out of this Guide
To get the most out of this guide, we suggest that you start reading and performing the step-by-step Getting Started tutorial. This tutorial will show you how create a set of surfaces. Once you have finished, you should move on to the Basic Tasks and Advanced Tasks sections, which deal with handling all the product functions. The Workbench Description section, which describes the FreeStyle workbench, and the Customizing section, which explains how to set up the options, will also certainly prove useful. Navigating in the Split View mode is recommended. This mode offers a framed layout allowing direct access from the table of contents to the information.

Accessing Sample Documents
To perform the scenarios, sample documents are provided all along this documentation. For more information on accessing sample documents, refer to Accessing Sample Documents in the Infrastructure User's Guide.

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Conventions
Certain conventions are used in CATIA, ENOVIA & DELMIA documentation to help you recognize and understand important concepts and specifications.

Graphic Conventions
The three categories of graphic conventions used are as follows:
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Graphic conventions structuring the tasks Graphic conventions indicating the configuration required Graphic conventions used in the table of contents

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Graphic Conventions Structuring the Tasks
Graphic conventions structuring the tasks are denoted as follows: This icon... Identifies... estimated time to accomplish a task a target of a task the prerequisites the start of the scenario a tip a warning information basic concepts methodology reference information information regarding settings, customization, etc. the end of a task

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functionalities that are new or enhanced with this release allows you to switch back to the full-window viewing mode

Graphic Conventions Indicating the Configuration Required
Graphic conventions indicating the configuration required are denoted as follows: This icon... Indicates functions that are... specific to the P1 configuration specific to the P2 configuration specific to the P3 configuration

Graphic Conventions Used in the Table of Contents
Graphic conventions used in the table of contents are denoted as follows: This icon... Gives access to... Site Map Split View mode What's New? Overview Getting Started Basic Tasks User Tasks or the Advanced Tasks Workbench Description Customizing Reference Methodology Glossary

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Index

Text Conventions
The following text conventions are used:
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The titles of CATIA, ENOVIA and DELMIA documents appear in this manner throughout the text. File -> New identifies the commands to be used. Enhancements are identified by a blue-colored background on the text.

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How to Use the Mouse
The use of the mouse differs according to the type of action you need to perform. Use this mouse button... Whenever you read...

What's New?
New Functionalities
Creating Associative 3D Curves on a Cloud of Points Working with a 3D Support Selecting Using a Filter Manipulating Light Sources

Enhanced Functionalities
Matching Curves Possibility to match both ends of a curve An automatic conversion is now possible when selecting a frozen curve or a non-Nurbs curve as input The Keep original is now available from the FreeStyle Dashboard Matching Surfaces The support detection capability is now available Performing a Symmetry on Geometry You can now select an axis system as the element to be transformed by symmetry Checking Connections Between Surfaces In Quick mode, possibility to analyze from one to three continuity types at once New Information button to hide or show minimum and maximum value tags Analyzing Distances Between Two Sets of Elements Possibility to relimit the discretized curve Possibility to calculate a minimum distance using Knowledge Performing a Surfacic Curvature Analysis On the fly analysis allowed even if the viewer mode is not set to Material Minimum and maximum curvature directions are displayed when performing on the fly analysis New Absolute / Radius Mode analysis options You can now define the default units that display during the analysis Creating a Temporary Analysis Automatic selection of the analyzed element for a stacked analysis Selecting a Support It is now available with the Match Surface functionality You can create a feature whose inputs belong to two different parts: an import is performed in the current part

this scenario should take about 15 minutes to complete. Profiler & Optimizer
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Getting Started
The following tutorial aims at giving you a feel of what you can do with FreeStyle Shaper & Optimizer. The final surface element will look like this:
.FreeStyle Shaper. It provides a step-by-step scenario showing you how to use key capabilities. The main tasks proposed in this section are: Starting the FreeStyle Workbench Creating a First Surface Editing the Surface Creating a Second Surface Creating a Blend Between Surfaces Applying a Global Deformation
All together.

The workbench looks like this:
from the
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Starting the FreeStyle Workbench
The first task will show you how to enter the FreeStyle Shaper workbench.
1. Choose FreeStyle from the Start -> Shape menu. The FreeStyle Shaper workbench is displayed and ready to use.FreeStyle Shaper. The only pre-requisite for this task is to have a current CATIA V5 session running. or click the FreeStyle icon Welcome to CATIA V5 dialog box.

remove the specification tree clicking off the View -> Specifications Visible menu item or pressing F3.FreeStyle Shaper. Profiler & Optimizer
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If you wish to use the whole screen space for the geometry.
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Select the Planar patch icon
2. and drag the mouse. one of its corner located where you clicked in the document. Right-click in the document and choose the Edit Orders item from the contextual menu. that is centered around the point you clicked. Set it to 5 for along U. A surface outline appears as you drag the pointer.FreeStyle Shaper.
3. Two values are displayed on the outline.
Use the Ctrl-click capability if you want the middle of the patch to be centered on the axis origin. Click anywhere in the workbench. 1. Click Close when finished defining these parameters.
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Creating a First Surface
The first task will show you how to create a single-patch planar surface in the current plane. indicating the length and width of the patch.
You can now define the degree of the mono-patch surface along U and V from the Orders dialog box.
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Editing the Surface
This task will show you how to modify the surface you just created.
2. 1. control points and mesh lines are displayed. or to set continuity constraints on the surface edges.
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Support: defines the type of translation to be applied. allowing to modify the U. Deformation can also be done using the Tuner dialog box displayed using the Edit contextual command on control points or mesh lines. refer to FreeStyle Settings.
The Control Points dialog box is also displayed: Use it to define the type of operation to be performed on the control points. They are used to manually pull on the surface so as to deform it. For further details. Select the surface. Depending on the settings. V orders.FreeStyle Shaper. Law: defines the type of deformation that is to be applied when several control points
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. Click the Control Points icon
As soon as you clicked the icon.

They represent the directions in which you can perform a deformation. Move the pointer onto one of the control points or mesh lines. Move selected points identically b.FreeStyle Shaper. 5. Arrows automatically appear.
The compass is oriented likewise:
4. Stretch selected points
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In P1 one mode you cannot choose the support (Translation in the plane is selected by default) and only two laws are available: a.
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have been selected. Move onto the center mesh line and pull the bottom arrow down. Right-click the compass and choose the Make YZ the Privileged plane.

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The selected control points are moved according to the translation type and law defined in the Control Points dialog box.
6.FreeStyle Shaper. Click a specific point to deform the surface at this point only.
. The same applies to mesh lines. By default all control points and mesh lines are selected.key while clicking (multi-selection capabilities). or select a set of points using the Ctrl-key or Shift. Click OK in the Control Points dialog box to accept the modified shape of the surface.

in
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Creating a Second Surface
In this task you learn to blend two surfaces. Select the new surface. right-click to display the contextual menu.
. 2. The second surface is created. and choose the Properties menu item to display the Properties dialog box.FreeStyle Shaper. 4. Successively click the four corner points of the first surface. 1. while specifying the continuity type. that is create one surface connecting both initial surfaces. change this surface's color using the arrow in the Color chooser. From the Graphic tab. Click the 4 Points Patch icon the Surface Creation menu to create another surface.

Move the pointer over the horizontal axis till it becomes red. Click OK in this dialog box. When the pointer changes to a cross. Repeat this operation with gliding the surface down along the vertical axis.FreeStyle Shaper. then grab the compass center and bring the compass over the 3-axis system at the bottom right-
. and glide the surface away from the first one.
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7. Move to the compass. press and hold while dragging the compass onto the new surface. Profiler & Optimizer
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5. The newly created surface is clearly identifiable.

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corner of the document.FreeStyle Shaper. The compass is set back to its default position.

2.FreeStyle Shaper. while specifying the continuity type. The Blend Surface dialog box is displayed. that is create one surface connecting both initial surfaces. Select the edge of the initial surface closest to the second surface. 1.
. The boundary is highlighted. Select the edge of the second surface closest to the initial surface. Profiler & Optimizer
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Creating a Blend Between Surfaces
In this task you learn to blend two surfaces. Click the Freeform Blend Surface icon . A blend surface is automatically computed. 3.

End of the Getting Started in P1 mode.
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4. Click OK in the Blend Surface dialog box to validate the blend surface.

1. use the default option: Intermediate surface use. defined in the plane indicated by the compass.
. then successively select all three surfaces. you want to modify all three surfaces according to a modification pattern you define in space. Now that both surfaces are linked. keeping all defined curvature continuities. The Control Points dialog box displays. It represents the planar patch. Click the Global Deformation icon . 3. In this case. Click Run in the Global Deformation dialog box to accept the deformation parameter definition.
2. A patch with control points and mesh lines is displayed. Press and hold the Ctrl-key. Profiler & Optimizer
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Applying a Global Deformation
This command is only available when using FreeStyle Optimizer.
The 3D compass is displayed along with the Global Deformation dialog box into which you can specify deformation options: using an intermediate patch or an axis use. equivalent to the same bounding box as the selected surfaces.FreeStyle Shaper.

. The space transformation is defined between the initial patch and the deformed patch. Do not change the options and click OK in the dialog box.FreeStyle Shaper. Profiler & Optimizer
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4.
The final deformed surface looks like this. Use the control points and the mesh lines of the planar patch to deform it. 5. All surfaces are automatically and dynamically deformed according to this intermediate patch deformation.

. Select Part in the List of Types field and click OK.
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This task shows how to open a new CATPart document and activate the FreeStyle Shaper workbench. 1.
The FreeStyle Shaper workbench is loaded and a CATPart document is opened.
2. allowing you to choose the type of the document you need.FreeStyle Shaper. Profiler & Optimizer
Opening a New CATPart Document
icon). 3. Select the File -> New commands (or click the New
The New dialog box is displayed. Choose Shape -> FreeStyle from the Start menu.

It lets you concentrate the design effort on establishing the proper design specifications. This specification tree can be customized using the Tools -> Options menu item. ultimately accelerating the design process. remove the specification tree clicking off the View -> Specifications menu item or pressing F3.
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. while leaving it to the system to compute or update the resulting geometry when required. Remember that these commands can also be accessed from the menu bar. Profiler & Optimizer
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The FreeStyle Shaper workbench document is made of: q the specification tree and the geometry area in the main window
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specific toolbars (geometry creation and modification toolbars. It would automatically open a new CATPart document. which captures and reuses process specifications. You could also directly choose FreeStyle from the Start menu. analysis toolbar) a number of contextual commands available in the specification tree and in the geometry.FreeStyle Shaper.
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If you wish to use the whole screen space for the geometry. Tree tab.
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The specification tree is a unique specification-driven and generative tool.

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Importing and Exporting Files
CATIA Version 5 includes unique two-way interoperability with CATIA Version 4 data, thus allowing CATIA Version 5 to benefit from the breadth of the CATIA Solutions Version 4 portfolio. CATIA Version 5 data can be loaded and processed in a CATIA Version 4 session. Similarly, CATIA Version 4 data can be read in a CATIA Version 5 session and converted to a CATIA Version 5 format for further edition. Refer to the CATIA V4 Integration User's Guide for further details on how CATIA Version 4 and Version 5 interoperate. 3D data exchange and more specifically surfaces exchange between CATIA Version 5 and other CAD systems can be done through Initial Graphics Exchange Specification (IGES) format. These exchanges are documented in the Interfaces User's Guide (Importing and Exporting External Files), as they are not specific to the FreeStyle Shaper workbench, but rather to the .CATPart document type. Therefore, refer to this chapter for a description of the specific surface elements that can be imported from or exported to the IGES Standard.

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Creating and Managing Curves
This chapter deals with curve creation and management using the FreeStyle Shaper workbench.

See also the FreeStyle Dashboard tools as they affect the curve creation and modification. Create associative 3D curves: specify the curve creation mode (passing through specific points, specifying the curve degree and smoothing the curve through points, or defining the curve control points), and click in space to indicate the curve definition points. Creating associative 3D curves on a scan: select one or more scans, specify the curve creation mode and click in space to indicate the curve definition points. Creating associative 3D curves on a cloud of points: select points on the cloud to indicate the curve definition points. Create free form curves on surfaces: select a surface, specify the curve creation mode (interpolation or smoothing in relation to the selected points), click definition points on the surface, double-click to end the curve. Project curves: select a curve, the surface on which it is to be projected and specify projection parameters Create blend curves: select two curves, activate their options display and use the contextual menu on the displayed text to modify the continuities and tension, manipulate the control points to define the blending point. Create a styling corner: select two curves, set the radius value. Match curves: select two curves, activate their options display and use the contextual menu on the displayed text to modify the continuities and tension, manipulate the control points to define the matching point. Edit curves using control points: select a curve, set the deformation options, pull on the control points in specific directions Smooth curves: select a curve or points on a curve, set the smoothing weight and click Run. Extrapolate curves: select a curve, specify the extrapolation mode, and enter the extension value. Extend curves: select a curve, specify the extension mode, and enter the extension value. Trim curves: select a curve, or point on a curve, and specify the breaking options Concatenate curves: select a multi-cell curve and set the tolerance value Fragment curves: break a multi-arc curve into several mono-arc curves Approximate/segment procedural curves: select a curve, specify the approximation tolerance, and resulting curve maximum orders and/or segments.

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This task explains how to create a 3D curve that is associative meaning you can add or delete points (whether control points or passing points) both at creation time or when editing. These curves can be created in space or lie on a geometrical element, or both. When the curve lie on a geometrical element and the later is modified, the curve is updated automatically, provided you choose the Automatic update option in Tools -> Options -> Mechanical Design -> Assembly Design -> General tab.
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Selecting all 3D points Editing Keeping a point Imposing a tangency constraint Imposing a curvature constraint Setting as arc limit

Through points: the resulting curve is a multi-arc curve passing through each selected point.

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Control points: the points you click are the control points of the resulting curve

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Near points: the resulting curve is a single-arc, with a set degree and smoothed through the selected points.

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You can edit the order by right-clicking the displayed text (displayed using the U, V Orders icon from the FreeStyle Dashboard or the Order option from Tools -> Options menu, Shape -> FreeStyle -> General tab), and choosing a new order value.

The Automatic order option enables you to automatically compute an order that will respect at best all the curve constraints. The computed value is displayed near the Auto tag.

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The Deviation option enables the user to set the maximum deviation between the curve and the construction points.

The result is a set degree through the selected points.

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The Segmentation option enables the user to set the maximum number of arc limits. These arcs are construction points and are inserted into the curve automatically. The minimum value is set to 1. The Max Order option enables you to set a bound for the computation of a mono-arc curve. This option is only available with the Control Points and the Near Points types (provided the Automatic Order is selected). r Control Points: when the Max order value is exceeded, the mono-arc curve becomes a multi-arc curve. As a consequence, the Max order value is no longer taken into account, as arcs have always 6 as order.
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Near Points: you cannot create a 3D curve with an order higher than the Max order value. The Max order value is always taken into account, whatever the result (mono-arc or multi-arcs curve).

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The minimum value for the Max order option is set to 5 for Control Points and 2 for Near Points. If the value defined in Tools -> Options -> Shape -> FreeStyle is set to 5, then, for Control Points, the Max order value is 6 (minimum and maximum bounds must be different). The maximum value for the Max order is the same as defined in Tools -> Options -> Shape -> FreeStyle. If you decrease the value in Tools -> Options and it is lower than the Max order value, then the latter value prevails.
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Smoothing options are now available to parameterize the curve:

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Chord Length (default parameterization) Smoothing parameter = 0

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Uniform Smoothing parameter = 0

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Smoothing parameter: enable a better control points distribution of the smoothed curve.

Smoothing parameter = 50

Smoothing parameter = 130

Deviation, Segmentation, and Smoothing options are only available for the Near Points creation type.

3. Move the pointer over a point. A manipulator is displayed allowing you to modify point location as you create the curve. By default, this manipulator is on the last created point. A contextual menu proposes several options to construct the 3D curve. Right-click on the manipulator to display the contextual menu. From then on you can choose the Edit item to display the Tuner dialog box and enter space coordinates for the selected point, or choose the Impose Tangency item to set a tangency constraint on the curve at this point. 4. Click the Insert a point icon box. The curve freezes. 5. Click the segment, between two existing points where you wish to add a new point and click the point location. within the dialog

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Once the point has been created, you are back to the edition capabilities on the curve.

6. Click the Remove a point icon

within the dialog

box, and select one of the existing points. The curve is recomputed immediately without the selected point.

7. Click the Free or constrain a point icon

within the dialog box, then select the point.

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If the point is a point in space (free), move the pointer close to the point or a wire to which it should be linked. You can then move the pointer over a geometric element and:
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move the point to the indicated point by clicking press and hold the Control key (Ctrl) to project this point onto this element according to the shortest distance from the point initial location.

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If the point was lying on another point or a wire (curve, line, spline, and so forth), it is freed from its constraint onto this element, and can be moved to any new location in space.

You can snap a point onto a surface using the Free or constrain a point icon. The point will be lying onto the surface, but not constrained. It can be moved using the manipulators. 8. Click OK to create the curve. A 3DCurve.xxx appears in the specification tree.

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Check the Disable geometry detection button, when you need to create a point close to a geometric element yet without constraining it onto the existing geometry. Check the Hide previsualisation curve to hide the previsualisation curve you are creating.

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Selecting all 3D points
It is possible to select all the points either in the specification tree or directly in the geometry. The Select all points contextual menu is available within the 3D curve action only, when the 3D Curve dialog box is open.
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In the specification tree: r select the geometrical set just by clicking it, or
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right-click the geometrical set and choose Select all points in the geometrical set from the contextual menu, or select a point in the geometrical set, right-click it and choose Select all points in the geometrical set from the contextual menu.

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In the geometry: select a point, right-click it and choose Select all points in the geometrical set from the contextual menu.

Contextual Options

Double-click your curve, right-click on the manipulator to display the contextual menu.

According to the creation type, the following options are available: Through Points Edit Keep this point Impose Tangency Impose Curvature Set as Arc Limit Remove this point Constrain this point X X X X X X X X Control Points X X Near points X X X X X X X

Editing

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1. Right-click any of the manipulators, and choose the Edit contextual menu to display the Tuner dialog box. This option allows you to redefine the tangency position, and its vector's step.

The Relative check box enables you to redefine the tangency relative position, and its vector's step. The Reset Origin button allows you to reset the origin of the relative position.

Keeping a point
1. Right-click an existing point and choose the Keep this point menu item to create a point at this location. A datum Point.xxx appears in the specification tree. You can create a Point.xxx either on each control point or on the selected control points.

Imposing a Tangency Constraint
Automatic Constraint

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When a curve is created in Through points or Near points mode, and its first point is constrained on any point of another curve, the new curve automatically is tangent to the curve on which its first point is constrained. As soon as the curve's second point is created, the imposed tangent is displayed on the new curve. To deactivate the default option, uncheck the Impose Tangency contextual menu on the tangent vector.

Tangency Constraint on Points

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When creating a 3D curve, you may want to impose tangency constraints on specific points of the curve. Then if you move the point at which a tangency constraint has been set, the curve will be recomputed to retain this tangency constraint at the point's new location. Depending on the creation mode, you can impose this constraints on a limited number of points: q In Through points mode: tangency can be imposed on any point
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In Near points mode: tangency can be imposed independently on each end points only In Control points mode: no tangency constraint can be imposed (end points can be constrained on other elements as described in step 7 above. See also Constraining a Control Points Curve.

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Here is how to do it: Open the 3DCurve1.CATPart document. 1. Move the pointer over an existing point, double-click it (the 3D curve dialog box appears), then right-click and choose the Impose Tangency menu item.

Two sets of manipulators are displayed: q two arrows representing the normed directions (vectors) of the tangency
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circles representing manipulators for this vector

You can also modify the tangency constraint by: q pulling the arrow
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gliding the circles double-clicking the arrow to invert the tangency direction

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You can set the tangency length by clicking on the arrow then dragging the mouse.

Right-clicking on any of the manipulators, you can also choose to define the constraint according to an external element: q Use current plane orientation (P1)/Use compass normal (P2): the tangency constraint is defined in relation to the normal to the current plane, possibly defined by the normal to the compass main plane When several points are constrained on the compass, all are modified if the compass settings are changed. When this option is checked, the direction cannot be modified directly using the vector manipulator, but only using the compass.

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Constrain on element: available only when a point is already constrained on a curve. The curve being created/modified becomes constraint in tangency or curvature to the constraining curve at this point. r Tangency constraint: in this case you can only modify the vector's norm using the Edit contextual menu, and no longer the vector's direction, the latter being defined by the constraining curve.
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Curvature constraint: in this case you neither modify the vector's norm using the Edit contextual menu, nor the vector's direction, the latter being defined by the constraining curve.

By default, when the tangency vector is constrained onto another curve, its initial direction is retained.

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Snap on elements: the vector's direction is defined by an external element. Grabbing a manipulators, you drag the pointer over a curve, and the curve becomes tangent to the curve detected by the pointer.

If the pointer is over a point the direction is computed as the line going from the constrained point and the detected point. If the pointer is over a plane, the tangency is defined by the normal to this plane.

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When snapping on an element, use the Control (Ctrl) key to obtain an exact snap, taking into account both the detected element and the vector's norm. Use the Shift key as a shortcut to activate/de-activate the Snap on elements option when passing the pointer over geometric elements.

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Control Points Curve Constraint

Once you are satisfied with the tangency constraint you imposed, simply release the manipulator and move the pointer around to recover the curve preview indicating that you are ready to create a new point.

Even though you cannot impose a tangency constraint on a curve created in Control points mode, you can constrain its end points on another curve, as described in step 7 above.

Right-click the text to display the contextual menu from which you can choose another continuity type: tangency.
Note that: q in Point continuity. or curvature. If you try to do so. Nevertheless. Profiler & Optimizer
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When setting a constraint on an end point. where applicable. you can add/remove points directly after the constrained end point.
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Imposing a Curvature Constraint
Right-click an existing point and choose the Impose Curvature menu item. Modifying the vector direction modifies the curvature direction. a warning message is displayed. A Continuity warning is displayed when trying to move the manipulators in a direction that is not compatible with the set constraint. An arrow representing the curvature direction (vector) is displayed. using the manipulators. a text is displayed indicating the type of continuity between the two curves.FreeStyle Shaper. The direction of the curvature is constrained in the plane defined as normal to the tangent vector. the selected point and the next two points are constrained
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This means that these second and third points will be modified if you move the constrained point along the constraining element. and the system resets the points as second and third points to be affected by the constraint. only the selected point is constrained
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in Tangent continuity. However. the selected point and the next one are constrained in Curvature continuity. you cannot constrain these points. because they are considered as already constrained.

This option is only available for the Near points creation type. you must ensure that a tangency continuity already exists. To do this. temporary analysis. Profiler & Optimizer
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To impose a curvature continuity. See Managing the Compass.
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Setting as Arc Limit
Right-click an existing point and choose the Set As Arc Limit menu item to start/stop an arc limit on this point.
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Available capabilities from the Dashboard. and/or specified through the FreeStyle Settings. you need to add a point before the end point. and furtive display. then move the end point to a new location. You cannot add a point past the end points. The creation plane for each free point is defined according to the current plane/compass orientation on the previous point. This option is only available for the Through points and Near Points creation type. The curve will pass through this point. are: datum creation. multi-select.FreeStyle Shaper.
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Use the F5 key to move the manipulators into a different plane of the compass. and de-select any combination of control points on these curves.
. by setting a new current plane/compass orientation on several points. move the new point where the end point lies. Use the standard shortcuts (Ctrl and Shift keys) to select. attenuation. Therefore you can change creation planes within the same curve. auto detection (except for Snap on Control Point option).

Choose the curve creation type. with a set degree and smoothed through the selected points. either graphically. 2. In that case.FreeStyle Shaper. In that case all points of the scan are taken into account even if you do not activate the Select all points menu. or after entering the 3D curve action.
The 3D curve dialog box is displayed. you can select only one scan. use the contextual menu Select all points to create a 3D curve on all the points of the scan. 1. you can select one or more scans.
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Control points: the points you click are the control points of the resulting curve
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Near points: the resulting curve is a single-arc. In that case.
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Open the 3DCurveOnScan1. Profiler & Optimizer
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Creating Associative 3D Curves on a Scan
This task explains how to create a 3D curve on a scan:
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either before entering the 3D curve action. In that case.CATPart document.
. Click the 3D Curve icon .
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Through points: the resulting curve is a multi-arc curve passing through each selected point. or from the specification tree.

i. it appears when the 3D Curve dialog box is open.e. q Right-click the Scan on Cloud.xxx appears in the specification tree.
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Right-click the cloud and select Select all points in the scan.
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A 3DCurve.
Selecting all points in a scan of cloud
It is possible to select a scan of cloud either in the specification tree or directly in the cloud from the contextual menu: The Select all points contextual menu is available within the 3D curve action only. Click OK to create the curve.FreeStyle Shaper. please refer to the Creating Associative 3D Curves chapter.
For further information on the options of the dialog box. Profiler & Optimizer
3.
Here is an example with Through Points
Contextual Options
.xxx in the specification tree and select Select all points in the scan.

you need to add a point before the end point. To do this. auto detection (except for Snap on Control Point option). Therefore you can change creation planes within the same curve. temporary analysis.
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Available capabilities from the Dashboard. and de-select any combination of control points on these curves. You cannot add a point past the end points. attenuation. Use the standard shortcuts (Ctrl and Shift keys) to select.
. See Managing the Compass. by setting a new current plane/compass orientation on several points. and furtive display. then move the end point to a new location.FreeStyle Shaper. and/or specified through the FreeStyle Settings. Please refer to the Creating Associative 3D Curves to get the corresponding information.
Only scans of the type "scan on cloud" can be selected since other types of scans might contain too many points. multi-select. move the new point where the end point lies. Profiler & Optimizer
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Double-click your curve. right-click on the manipulator to display the contextual menu.
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Use the F5 key to move the manipulators into a different plane of the compass. are: datum creation. The creation plane for each free point is defined according to the current plane/compass orientation on the previous point.

1. Click the 3D Curve icon .FreeStyle Shaper. 2. Choose the curve creation type. Profiler & Optimizer
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Creating Associative 3D Curves on a Cloud of Points
This task explains how to create a 3D curve using clouds of points or polygons as support.
The 3D curve dialog box is displayed. The curve may not lie on the cloud or polygons but its construction points should be constrained onto them: the manipulator is always tangent to the cloud or polygon and always lie on it.CATPart document. Open the 3DCurveOnCloud1.
.

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Through points: the resulting curve is a multiarc curve passing through each selected point. with a set degree and smoothed through the selected points.
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Control points: the points you click are the control points of the resulting curve
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Near points: the resulting curve is a single-arc.
.FreeStyle Shaper.

The Select all points contextual menu is available within the 3D curve action only.
Selecting all 3D points
It is possible to select all the points either in the specification tree or directly in the geometry.
For further information on the options of the dialog box. A 3DCurve.
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If the cloud is tessellated. Therefore.xxx appears in the specification tree. please refer to the Creating Associative 3D Curves chapter. when the 3D Curve dialog box is open. points of the resulting curve are constrained on both cloud and points of cloud. or
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right-click the geometrical set and
. Click OK to create the curve. points of the resulting curve are constrained on the cloud but not on the points of the cloud. you must snap from point to point on the cloud. Therefore. Profiler & Optimizer
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3.
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If the cloud is not tessellated. you can select a point anywhere on the cloud.
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In the specification tree: r select the geometrical set just by clicking it.FreeStyle Shaper.

auto detection (except for Snap on Control Point option).FreeStyle Shaper. right-click it and choose Select all points in the geometrical set from the contextual menu. rightclick on the manipulator to display the contextual menu.
. Therefore you can change creation planes within the same curve. move the new point where the end point lies. Use the F5 key to move the manipulators into a different plane of the compass. multi-select. Profiler & Optimizer
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choose Select all points in the geometrical set from the contextual menu. and de-select any combination of control points on these curves. and furtive display. rightclick it and choose Select all points in the geometrical set from the contextual menu.
Contextual Options
Double-click your curve. temporary analysis. or
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select a point in the geometrical set. by setting a new current plane/compass orientation on several points. See Managing the Compass. You cannot add a point past the end points.
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In the geometry: select a point. attenuation. To do this. then move the end point to a new location. are: datum creation. you need to add a point before the end point. The creation plane for each free point is defined according to the current plane/compass orientation on the previous point. Note that you cannot constrain on an element when imposing a tangency or curvature constraint. and/or specified through the FreeStyle Settings. Use the standard shortcuts (Ctrl and Shift keys) to select.
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Available capabilities from the Dashboard. Please refer to the Creating Associative 3D Curves to get the corresponding information.

with a set degree and smoothed through the selected points.
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. the resulting curve is a multi-arc parametric curve passing through each selected point. Profiler & Optimizer
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Creating Free Form Curves on Surfaces
This task explains how to create trimming curves on a surface. Open any document containing a surface from the samples directory.
The Options dialog box is displayed letting you choose the curve type: an isoparametric curve. or the CurveOnSurface1. the points you click are the control points of the resulting parametric curve. or isoparametric curves.
Point by Point
If you choose the Point by point creation type. as if you were using the editing capabilities (see Editing Curves Using Control Points).
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If you choose to use the Through Points mode. Select the surface on which the curve is to be created. you need to define the curve creation mode: by interpolation or smoothing. If you choose the Near Points mode. Click the Curve on Surface icon . but do not need to divide it.FreeStyle Shaper.
2. the resulting curve is a single-arc parametric curve.CATPart document. 1. Two types of curves are available for creation: freeform curves passing through all points you click. If you choose the With control points mode. or a user-defined curve (Point by point). This is the default value. These curves must lie on the surface.

A dot is displayed identifying the starting point location on the surface. therefore clicking anywhere on the surface lets us define a point on its edge.FreeStyle Shaper. you can move the pointer above any of the creation points and pull on the manipulators up to the surface edges. For example. In the illustration.
. using the manipulators on the control points. Choose a mode and click anywhere on the selected surface. Click as many locations as you wish the curve to go through.
Capabilities are available from the contextual menu when right-clicking a contact point. You can modify the shape of the curve at any time while it is being created. and the curve is previewed as you move the pointer around.
2. Profiler & Optimizer
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1. Dots are displayed where you clicked. the Auto detection mode is active to Snap On Edge icon ( from the
Dashboard).

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Any surface can be used. If you choose the Near Point option.FreeStyle Shaper. while being in the command.
The surface can now be used for other purposes. in both U and V directions. The curve end point can be anywhere on a surface or on an edge.
Click the Break icon
and select an
area delimited by the curve to trim the initial surface (see Redefining Surface Limits).
. following its shape. or click OK. check the Order option fr
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Isoparametric
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Manual selection: you can create as many isoparametric curves as necessary. whether planar or previously deformed. Double-click to create the end point of the curve the surface. Profiler & Optimizer
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3. The curve has been created on the selected surface. such as trimming the surface. for example.

while being in the command. perform the same operation to create the second curve.
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Each created curve can be independently modified using the 3D manipulators.
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Automatic selection: you can create as many isoparametric curves as necessary. You can select the Invert Parameter option to inverse the direction of the curve.
2. 3.
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1. Run the mouse on the surface and click to create the curve. Capabilities are available from the contextual menu when right-clicking a contact point. Still in the command.FreeStyle Shaper. in both U and V directions. The curves have been created on the selected surface. Click OK.

2.FreeStyle Shaper.
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Each created curve can be independently modified using the 3D manipulators. Continue creating the curve as usual
. The curves have been created on the selected surface. Click OK. Profiler & Optimizer
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1. 3. You can select the Invert Parameter option to inverse the direction of the curve. Define the value for U and V directions. Click the surface to preview the created curves. Use the With control points option and click the first two points on the surface edge (parametric line).
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Creating a tangent curve:
a. Capabilities are available from the contextual menu when right-clicking a contact point. b.

finish as usual. if you wish to make it tangent on both sides of the surface. proceed by clicking two points on the other edge
d.
. by clicking the last point on the surface edge. The surface edge presents a tangency continuity.
This is especially useful when breaking a surface. Profiler & Optimizer
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c.FreeStyle Shaper.

To facilitate the edge detection.
.FreeStyle Shaper. even if you modify them using the control points capability after creation time. Available capabilities from the Dashboard. auto detection. are: datum creation. and contact points. Profiler & Optimizer
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The resulting curves will always lie on the surface. use the remote auto detection capability. for example. and/or specified through the FreeStyle Settings.

2. Select a curve. Profiler & Optimizer
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Projecting Curves
This task explains how to project curves on surfaces.
The projected curves are displayed. Click the Project Curve icon . Press the Ctrl key and select the surface or set of surfaces on which the curve should be projected.FreeStyle Shaper.
The Projection dialog box is displayed. in dashed green. Choose the projection orientation from the Projection dialog box:
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Projection Normal to the Surface Projection According to the Compass
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4. 1. on the target surface along some information:
. Open the ProjectCurve1.
3.CATPart document.

then clicking OK.
.FreeStyle Shaper. The Converter Wizard is automatically used to process the resulting curve and generate either a 2D NUPBS (Non Uniform Polynomial B-Spline) curve identified by the Exact text. The Converter Wizard is then explicitly launched allowing you to control the new curve creation. or a 3D NUPBS curve (identified by Cv text). If you wish to further control the projected curve. and show up in the specification tree as two different elements. right-click the displayed text and choose the Edit contextual menu. Click OK in the Projection dialog box to create the projected curves. Profiler & Optimizer
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Projection according to the compass orientation
Projection according to the normal to the surface
The projected curves are BSplines lying on the surface.
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When you project a curve on two surfaces. there may be no tangency continuity. in the case of a 2D curve you may wish to generate a single segment curve by checking both the Segmentation and Single button in the Converter Wizard. For example. If you chose the projection according to the compass orientation.
5. two curves are created on the surface.

. The element's topology (for example a relimited curve or surface) is taken into account for the projection.
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Available capabilities from the Dashboard are: datum creation. and keep original.FreeStyle Shaper. Multi-cell curves can be selected: the resulting projected curve will also be a multi-cell curve.
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Check the Display Information option from the Converter Wizard's dialog box to the resulting curve's order and number of segments. Multi-selection of curves is allowed. Profiler & Optimizer
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Use the Furtive Display icon
to view the control
points on the projected curve (in blue).

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Creating Blend Curves
This task explains how to create blend curves. Blending means that a connecting curve will be created between two selected curves, taking certain continuity, position and tension constraints into account. Open the BlendCurve1.CATPart document. 1. Select two curves. 2. Click the FreeStyle Blend Curve icon .

The Blend Curve dialog box opens.

3. Select the second curve, in case you have not previously selected it. The blend curve is automatically previewed. By default it connects the curves at their end points closest to the selected points.

4. Make sure the Continuity icon is active in the Dashboard and right-click onto the identifier to edit the continuity constraint, using the contextual menu.

The default continuity type is Tangent. You can do the same on the other end point.

FreeStyle Shaper, Profiler & Optimizer
5. Make sure the Contact Points icon is active in the

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Dashboard, to display the contact points on the blend curve end-point. Capabilities are available from the contextual menu when right-clicking a contact point. 6. Move the pointer close to the contact point and drag the manipulator to modify the blend curve connection to the initial curves.

7. Still from the Dashboard, make sure the Tensions icon is

active, and modify the tension by sliding the displayed value along the green segment.

This segment represents the direction and limits of the blend curve tangent at its end points.

8. You can also edit the value, or invert the tension direction, using the contextual menu on the value.

FreeStyle Shaper, Profiler & Optimizer
Tensions are now homogenized between blend surfaces and blend curves, so that the borders of a blend surface have the same shape as the blend curves, providing they are built on the same supports.

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This homogenization is only possible with an approximated blend surface.

9. Once you are satisfied with the new curve, click OK in the Blend Options dialog box. The blend curve is computed .

The curve resulting from the blend remains selected by default. If you wish to perform analyses, make sure you select the other curves using the Ctrl-key. Available capabilities from the Dashboard, and/or specified through the FreeStyle Settings, are: datum creation, auto detection (Snap On Vertex option only), attenuation, continuity, contact points, tensions, and furtive display.

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Creating Styling Corners

This task explains how to create a styling corner, that is a connecting curve of a given radius between two other planar curves. Styling corners are especially useful to create good quality surfaces based on a curve net, as described in Creating a Net Surface (available with the FreeStyle Profiler product only). Open the StylingCorner1.CATPart document. 1. Click the Styling Corner icon The Styling Corner dialog box is displayed. 2. Select the two curves to be connected by a styling corner. 3. Key in a radius value. .

4. Click Apply.

The corner is previewed, with manipulators, at the circle center, the constant radius limit (the segment between the two solid radius lines), and at the contact points, provided this option is active in the dashboard.

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Capabilities are available from the contextual menu when right-clicking a contact point.

It may be interesting to perform a curvature analysis clicking the Porcupine Curvature Analysis icon to visualize the resulting corner's curvature, and possibly modify it using the corner's manipulators.

In this case, it may be useful to smooth the curvature at the contact points and reduce the constant radius area:

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5. Modify the options as needed:

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the Radius value in the editable field the Single Segment option to impose a limited number of control points for the corner curve, thus resulting in a single arc curve.

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In this case, the generative circle is not displayed, only contact points are, provided the Contact Points option is active in the dashboard. Depending on the radius value, there may be several solutions. In this case, you are prompted to select one of the proposed solutions. The concatenation mode (see below) is not available with this mode.
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the resulting curve type:

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a. Trim: to create a three-cell curve limited to the initial curves endpoints. You can display their control points independently if you use the Control Points icon (it creates another independent curve corresponding to the selected cell). Initial curves are duplicated and trimmed at the contact points with the corner segment.

b. No Trim: to create the corner arc only limited at the intersection with the initial curves Initial curves are not modified.

c. Concatenation: to create a mono-cell curve limited to the initial curves endpoints. You can display its control points independently if you use the Control Points icon (it creates

another independent curve corresponding to the whole curve). Initial curves are duplicated, trimmed at the contact points with the corner segment, and concatenated with the latter.

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6. Click OK to create the styling corner.

A useful application of this command is to create a set of styling corners based on intersecting curves, then create an associate net surface based on these styling corners. You can then modify the initial set of curves and the surface automatically is recomputed.

FreeStyle Shaper, Profiler & Optimizer

Matching Curves

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This task explains how to match a curve with another curve, a point on curve or a 3D point.. Open the MatchCurve1.CATPart document. 1. Select the curve you wish to match to another curve.

2. Click the Match Curve icon

.

The Match Curve dialog box is displayed.

3. Select the second element (first reference element) for the match curve to be joined to. It can either be:

1. a curve 2. a point on curve with history 3. a datum point on curve 4. a 3D point 5. a vertex

The first curve is automatically modified so as to be connected to the second element while taking the continuity type into account. The number displayed on the first curve (Nx) corresponds to number of control points on that curve.

1. Match between a curve and another curve

2. Match between a curve and a point on curve with history

3. Match between a curve and a datum point on curve

4. Match between a curve and a 3D point

5. Match between a curve and a vertex

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If you select a second reference element, both ends of the curve can be matched.

Two tags for each reference element are displayed near the matching curve extremities. Only one reference element is current, meaning that you can only manipulate the second extremity of the matching curve, while the other extremity is fixed. To be able to select another reference element to perform another match, you must click the corresponding tag.

To deselect the first reference element, you need to perform a local undo.
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If a curve is selected as the second element, all continuities can be applied (point, tangent, and curvature continuities) If a curve or a point on curve with history is selected as the second element, a point or curvature continuity can be applied. If a datum point on curve, a 3D point, a vertex is selected as the second element, a point continuity will be applied. If the second element to match (a point on curve with history, or a vertex) lies one more than one support, the Refer to the Selecting a Support chapter for further information. appears.

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The Project End Point option allows a linear projection of the minimum distance between two curves by projecting the initial curve onto the target curve.

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The Quick Analysis option enables to perform a violation diagnosis of the curve matching. The original degree is kept (it is no more automatically increased). Several parameters are taken into account between the two curves: r distance
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continuity degree curvature difference

r

4. Click Ok in the Match Curve dialog box to create the matched curve as it is previewed.

If you select a frozen curve (a curve with an history) or a non-Nurbs curve as input, a dialog box is issued warning you that an automatic conversion will be automatically performed before the matching operation: - if an exact conversion is possible, a new Nurbs curve will replace the input one in order to perform the match. This new curve will be added in the specification tree.

Make sure the Continuity icon is active
in the Dashboard and. the Converter Wizard panel appears allowing you to define the approximation according to a tolerance using parameters such as U. a warning message is issued. right-click onto the identifier to edit the continuity constraint. Profiler & Optimizer
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.
You can choose from the point.
. tangency or curvature continuity type to be taken into account. you can either:
.modify the continuity type by clicking it (it is displayed sequentially) or by selecting a type from the contextual menu. V orders.
In order to reach the correct degree (0 or 180 degree) and percentage (0%).if there is a deviation or no exact conversion exists. or
.FreeStyle Shaper. V orders icon
is
active in the Dashboard so that the numbers of control points are displayed.
2. Make sure the U.
Working with the FreeStyle Dashboard
1.
If a continuity type leads to some inconsistencies regarding the curve's original degree. using the contextual menu. and deviation tolerance. patch numbers.increase the number of control points by clicking the number (the value is increased by one) or by selecting a number from the contextual menu.

Click OK in the Break Options dialog box. and modify the tension by sliding the displayed value along the green segment.
6. attenuation. Profiler & Optimizer
3.FreeStyle Shaper. continuity. are: datum creation. thus interactively redefining the connection location.
A new split curve is created replacing the initial one. and/or specified through the FreeStyle Settings. Click OK in the Match Curve dialog box to create the matched curve as it is previewed.
8. tensions.
5. to display the point manipulators and to move the points along the curve. Make sure the Tensions icon
is active
in the Dashboard. and select the
7. Select the side to be removed. Available capabilities from the Dashboard. contact points.
4.
. If you wish to perform analyses. and furtive display. When working in P2 mode. click the Break Surface or Curve icon curve to be broken.
The curve resulting from the match remains selected by default. auto detection (Snap On Vertex option only). make sure you select the other curve using the Control key.
This segment represents the direction and limits of the match curve tangent at its end-points. Make sure the Contact Points icon is
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active in the Dashboard. Keep original.

the Converter Wizard is not displayed. and the curve is not a NUPBS curve (Non-Uniform Polynomial B-Spline). In this case.FreeStyle Shaper. when a curve can be exactly converted. the Converter Wizard will be automatically displayed when the curve cannot be exactly converted. However. Open the EditControlPoints1. Planes and lines are used to quickly orientate the compass in the control points command. the conversion is done automatically and a message is issued. along with the 3D compass and the curve degree. Control points and lines are displayed. the Exact text is displayed on the element for information. or line for example. or select a set of points using the Ctrl-key or Shift-key while clicking (multi-selection capabilities). By default all control points and mesh lines are selected. This allows you to control the conversion tolerance. Click the Control Points icon . it will modify the compass orientation. Click a specific point to deform the surface at this point only. Select the curve you wish to edit.
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. such as a spline.
2. Therefore if you select a plane or a line.CATPart document.
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If you select a curve that has been created outside the FreeStyle workbench. The same applies to mesh lines. Profiler & Optimizer
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Editing Curves Using Control Points
This task explains how to modify a curve using its control points. 1.

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Support defines the type of translation to be applied Law defines the type of deformation that is to be applied when several control points have been selected. refer to How to Use the Support and Law Options?
In P1 mode.FreeStyle Shaper. Profiler & Optimizer
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3. Move the pointer over a point or a line.
. Stretch selected points You cannot specify a Support. you can modify curves according to two laws only: 1. Move selected points identically 2. Arrows are displayed according to the Support and Law options active in the Control Points dialog box.
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For further information on supports and laws.

Use the Dashboard to display the order number directly on the curve. Use the contextual menu to choose the order number for the curve.
. Pull on the arrow matching the direction in which you want to deform the curve. Profiler & Optimizer
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4.
If you increase the order number to 11. 6.
5. V Orders icon. using the U.
The value is displayed on the curve.FreeStyle Shaper. Click OK in the Control Points dialog box to validate the modifications. the result is:
7.

It lets you define the ratio between the mouse displacement and the actual displacement of the manipulator. use the attenuation capability from the Dashboard. or continuity type. continuity constraints are not detected. V Orders icons (P2) or the specified settings (using the Tools -> Options -> Shape -> FreeStyle -> General tab) (P1). the following manipulation options are available:
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To fine-tune the manipulators.
Use the Manipulators (arrows) to modify the curve as it is created. If the Manual Update mode is activated in Tools -> Options -> Part Infrastructure -> General tab. To snap a point onto external geometry.FreeStyle Shaper. When selecting several curves.
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You can edit these by right-clicking the displayed text. In P2 mode.
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The following options are available in P2 mode only:
. To display the order number and continuity type directly on the curve. and choosing a new order number. Profiler & Optimizer
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Use the Control Points dialog box to modify the curve according to certain predefined laws. if a continuity constraint exists. use the auto detection capability from the Dashboard. the continuity tag displayed is set by default to the same continuity imposed by the constraint. choose the Inflections checkbox. This attenuation factor is saved in the CATIA settings. To perform a quick analysis of the mesh line inflection. use the Dashboard's the Continuity and U.

and Symmetry capabilities are only available with the FreeStyle Optimizer product. and attenuation. button of the Control Points dialog box: r Freezing of the selected points (no other can be selected) and of the Support option
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Dynamic display of the initial curve and of the delta as you pull on the control points Global selection/de-selection of control points using the Select All Select All icons. without having to click the geometry and De-
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The Projection. see Smoothing Curves.
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Capabilities are available: r from the contextual menu when right-clicking a control point. Profiler & Optimizer
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Further modification options are available from the More.
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To have further information about how to smooth curves. keep original. Smooth.FreeStyle Shaper.. specified through the FreeStyle Settings.
. are: datum creation.
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from the FreeStyle Dashboard.. auto detection.

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Smoothing Curves
This command is only available with the FreeStyle Optimizer. Click the Control Points icon
. and the Control Points dialog box appears.
Control points are displayed on the curve.FreeStyle Shaper.
. This task explains how to smooth curves.
2.CATPart document. Open the SmoothCurve1. 1. Select the curve to be smoothed.

Once you are satisfied with the smoothed curve obtained. and the curve is smoothed in this area only. press and hold down the Ctrl-key. Still maintaining the Shift-key down. 4.
You do not need to select the whole curve. Only the explicitly selected points are highlighted. and click Run. Define the smooth weight using the slider. You can locally smooth the curve. Profiler & Optimizer
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3. Simply use the multi-selection capabilities: q Press and hold down the Shift-key and click on a first point. then move on to the other points to be selected. The curve is smoothed according to the value. Click again to repeat the smoothing operation.
. click another point of the curve.
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Click a first point. click OK in the Control Points dialog box.
5.FreeStyle Shaper. and smoothing is performed on these points only. All points selected between the two selected points are selected as well.

It will be extrapolated on the end-point side closest to the selection point. that is by modification of its length.
3.
The Extrapolation dialog box is displayed.FreeStyle Shaper. 2. Profiler & Optimizer
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Extrapolating Curves
This task explains how to modify a curve.CATPart document. or surface boundary.
. Click the Tangential option: The curve is extrapolated taking into account the keyed in length (expressed in model units). Click the Styling Extrapolate icon . by extrapolation. Select the curve to be extrapolated. Open the Extend1. Here we keyed in 100. It can be a positive or negative extrapolation meaning that you can actually lengthen or shorten the curve. Only the Tangential extrapolation type is available for curves. 1.

.
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You can also use the manipulators to interactively modify the value. The curvilinear length of the extrapolation is displayed.FreeStyle Shaper. attenuation. Profiler & Optimizer
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If you key in a negative value. auto detection. Click OK to create the extrapolated curve. the resulting curve is created in the other direction.
5.
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the dashboard are: datum creation. Capabilities are available from: r the contextual menu when right-clicking an end point.

Open the Extend1. Use the manipulators to extend the curve on both sides. Two extension modes are available. Profiler & Optimizer
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Extending Curves
This task explains how to lengthen a curve by extension.
3. 1. Two working modes are available:
If you go over a curve's extremity with the mouse. In one case.
. Multi-selection of curves is now possible. the manipulator becomes the master manipulator.
The Extend dialog box is displayed.FreeStyle Shaper. Select the curve(s) to be extended. it is a positive parametric extension. or it can be an extension by addition of segments to the curve. Click the Extend icon . that is by modification of its length. meaning it is active at that extremity.
Manipulators are displayed on the curve.CATPart document. 2.

4. 2.
The distance tag displays the absolute curve distance from the extremity of the original curve..FreeStyle Shaper. the last segment (defined by the arc limits) is made longer. the new curve is computed from the original curve.
.
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With the Keep segmentation option unchecked: the curve is extended taking the curvature continuity of the last segment into account. not from the curve previously computed.
If you change the mode. Right-click the distance tag which displays the absolute curve distance. This means that only this last segment can be extended.
Extending Curves Using Absolute and Relative Distance Modes
1. Click OK to create the extended curve. When the value is positive. Profiler & Optimizer
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With the Keep segmentation option checked: use the manipulator to define the curve extension. Choose the Edit item in the contextual menu.

5. 4. Choose the Slave item in the contextual menu. The slave manipulator ''follows'' the master manipulator.FreeStyle Shaper. Here we chose 100mm. A symbol appears
near the slave manipulator and its distance tag is symbolized in yellow. Click Close to apply the new value.
. Now use the manipulators to extend the second curve. Enter the extension value. Again.
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This value is always positive. Profiler & Optimizer
The Edit Box dialog box is displayed.
7. 3. The manipulator becomes active and the distance tag is symbolized in green.
You can see that both curves are extended with the same delta (93. right-click the distance tag.432mm). 6. This option enables to apply the delta curve extension to the master manipulator and the slave manipulator.

Therefore the extended curve is made of two or more cells.
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You can also access these contextual menu items by clicking the distance tag and moving sequentially from one option to the other (Edit.FreeStyle Shaper.
. The Edit and Keep this point options are also available from the contextual menu when right-clicking the manipulator. then Free).
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You can extend a trimmed 3D or 2D curve: the parameterization of the original curve is used. then the extension is calculated. it becomes active again. The Free option enables to free the slave manipulator. Capability are available from the Dashboard: datum creation and keep original. a 3D cell is added. then Slave. Profiler & Optimizer
If you go over the distance tag of the slave manipulator with the mouse. When extending a 2D curve.

Choose the Break type by clicking on the icons on the left.CATPart document.
. Open the Break2.FreeStyle Shaper.
2. Three types are available:
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Curves by points Curves by curves Surfaces by curves (please refer to the corresponding chapter)
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Breaking Curves by Points
In the Selection page. Click the Break icon . 1.
The FreeStyle Break dialog box is displayed as well as the Break Report panel and the Tools Palette. the Cut (0) text is highlighted. Profiler & Optimizer
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Trimming Curves
This task explains how to trim curves by one or more curves or points.

Select one or more curves to be trimmed.
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1.FreeStyle Shaper.
. Click the Cutting (0) text and select one or more cutting points.

If you click on the text. etc). the corresponding curve is highlighted in green in the 3D geometry. If you click on the text. By default.FreeStyle Shaper. it means that the problem
. Click Apply. all elements are kept.
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the cutting elements that cannot be used for the Break (marked by the condition to be applied so that they can be used: projection.
The Break Report panel displays all the information regarding the cutting elements. It lists:
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the cutting elements that can be used for the Break (marked by a green tip). the corresponding curve is highlighted in red in the 3D geometry.
r
If there is no selection of cutting elements. Profiler & Optimizer
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3. an error message is issued and the Break Report panel informs you that no element is selected.
r
If a red cross is displayed.

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Keep all: all parts of the all curves are kept
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Keep all but this: all parts of all curves are kept except the selected one
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Remove all but this: all parts of all curves are removed except the selected one
. Profiler & Optimizer
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cannot be managed by the system.
4.
A contextual menu is available on the each part of the surface. Click the parts of the curves you do not want to keep: they appear dotted in the 3D geometry.FreeStyle Shaper.
This panel can also be opened via the Display tab.

the points that do not lie on the trimmed curves will not be projected onto the surface.FreeStyle Shaper. As a consequence.
Projection
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no projection: click the Projection text to make the projection optional. Click the <<Settings text to access advanced settings. The following options can be activated by clicking on the icons. they will be projected (pseudo-intersections) onto the curves according to the direction set in the Break dialog box. that is:
. Profiler & Optimizer
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5.
If certain points do not lie on the trimmed curves.

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Normal: click the normal icon so that the projection is normal to the element. Profiler & Optimizer
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Compass: click the compass icon so that the projection is normal to the compass. Here is an example with a projection normal to the compass.FreeStyle Shaper.
.
Relimitation
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Keep mesh: click the Keep mesh icon so that the curves are topologically relimited and the control points of the initial curves are kept.

FreeStyle Shaper. the Cut (0) text is highlighted. Here is an example with a projection normal to the compass.
1.
.
Breaking Curves by Curves
In the Selection page. Select one or more curves to be trimmed. Profiler & Optimizer
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Shorten mesh: click the Shorten mesh icon so that the curves are geometrically relimited and the control points of the resulting curves are kept.

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The Break Report panel displays all the information regarding the cutting elements.FreeStyle Shaper. the side of the curve to be extrapolated is circled in red.
r
If there is no selection of cutting elements. extrapolation. the corresponding curve is highlighted in green in the 3D geometry.
r
In case of an extrapolation problem. If you click on the text.
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the cutting elements that cannot be used for the Break (marked by the condition to be applied so that they can be used: projection. If you click on the text. an error message is issued and the Break Report panel informs you that no element is selected.
r
If a red cross is displayed. the corresponding curve is highlighted in red in the 3D geometry.
. etc). It lists:
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the cutting elements that can be used for the Break (marked by a green tip).

This panel can also be opened via the Display tab.
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Keep all: all parts of the surface are kept
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Keep all but this: all parts of the surface are kept except the selected one
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Remove all but this: all parts of the surface are removed except the selected one
. 2.FreeStyle Shaper. A contextual menu is available on the each part of the surface. Profiler & Optimizer
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it means that the problem cannot be managed by the system. Click the parts of the curves you do not want to keep: they appear dotted in the 3D geometry.
You can now cut the cutting elements.

Click the <<Settings text to access advanced settings. they will be projected onto the surface according to the direction set in the Break dialog box. that is:
Compass: click the compass icon so that the projection is normal to the compass
Relimitation
. The following options can be activated by clicking on the icons.FreeStyle Shaper. Profiler & Optimizer
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3.
Projection
If certain points do not lie on the trimmed curves.

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Click the Display>> text to manage the display of the 3D icons and the Break Report panel. keep original.
3. Available capabilities from the Dashboard are: datum creation.
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Shorten mesh: the curve is geometrically relimited and the control points of the resulting curve are kept.FreeStyle Shaper.
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. and temporary analysis. Click OK to trim the curves. Profiler & Optimizer
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Keep mesh: the curve is topologically relimited and the control points of the initial curve are kept. insert in a new geometrical set.

Select the curves you wish to concatenate and click Apply. provided the tolerance is compatible. If you are using the Auto Update Tolerance mode. Click the Concatenate icon The Concatenate dialog box is displayed. therefore no message is issued. 2. 1. and set the tolerance value to 1. the minimum tolerance value is automatically modified. a message is issued prompting you to increase it.FreeStyle Shaper.
Here we selected Join. However.
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Concatenating Curves
This task explains how to concatenate a 3D multi-cell mono-domain FreeStyle curve or separate contiguous curves into a mono-cell curve. Open the Concatenate1. If not. . no concatenated curve is previewed. The Maximum deviation value displayed in the dialog box (see step 4) is computed as the standard distance analysis and therefore is not necessarily the minimum tolerance value to be set in order to concatenate the curves.
A single curve is previewed. the minimum tolerance value necessary to obtain a result is then automatically displayed.
3. The resulting curve is a curvature continuous curve (C2). This document contains a two Join-type elements. to help you. each identified by different colors. with its segment limits.
Would the tolerance value you entered not be adequate. and the OK button is grayed. and a set of connex curves.
This value defines the maximum parametric deviation allowed between the selected elements and the resulting curve when concatenating.2 from the specification tree. Set the tolerance value.CATPart document.

FreeStyle Shaper. 6.
5. Check the Auto Update Tolerance option to automatically update the tolerance value in case the value you set is too low.
. Click More>> in the dialog box.
7. the maximum deviation is also indicated in the dialog box. Profiler & Optimizer
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4.
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If no resulting curve is displayed once you have clicked Apply. Check the Information option. The minimum value to enable the concatenation is displayed and the concatenation is performed. the result of the concatenation of the elements making up the initial Join. Click OK in the Concatenate dialog box. A curve is created. that is:
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N: number of control points o: the curve order s: the number of segments in the curve
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q
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the maximum deviation
In case you did not check the Information button. The corresponding information is displayed on the resulting curve. increase the tolerance value.

the Apply button is grayed. and you cannot create the concatenated curve. (Join. you can select several contiguous curves using the Control key.FreeStyle Shaper.
. and each one will generate a concatenated curve. Profiler & Optimizer
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Multi-selection is available using the Control Key.)
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Similarly.1 in green is still visible behind Curve. but you can notice the deviation due to the discontinuity of the initial element. you will need to increase the tolerance value accordingly. to generate a single curve. If the selected curves are not connex (if there is a gap between two curves). or a trap. you can select several Join elements for example.e. i.19. the maximum deviation will increase considerably. In this case too.
Set of independent connex curves
Resulting concatenated curve
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If the selected elements present a curvature discontinuity (as illustrated below).

In the example. 1. The Type frame does not apply for curves. in
The Fragmentation dialog box is displayed. we assigned a different color to each of the resulting mono-arc curves. This means that independent curves are created. Profiler & Optimizer
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Fragmenting Curves
In this task you will learn how to fragment multi-arc bodies into mono-arc bodies.CATPart document. The curve is fragmented in as many curves as there were arcs in the initial curve. 2.
4. Click the Fragmentation icon the Shape Modification toolbar. thus allowing the pre-visualization of the resulting curves. Select the curve.FreeStyle Shaper. Open the FragmentCurve1. Click the Keep original icon from
the Dashboard if you want to keep the initial curve when fragmenting the body. 3. Click OK.
. The selected curve is previewed with separators indicating the limits of each arc.

Open the Approximate1. In P1 mode. Otherwise. parabolas. On the geometry. created using other products but FreeStyle.FreeStyle Shaper.
The Converter Wizard dialog box is displayed allowing you to define the approximation according to a tolerance. and the Converter Wizard is not displayed. and to modify the number of arcs (segments) onto any curve. This is the often the case with splines and lines. Orders: that is the maximum allowed order along the U direction for each curve segment. including these created using FreeStyle products.CATPart document. the Max order is set to 16 and cannot be modified. This approximation is automatically performed when you try to edit a curve using control points.
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. it is done automatically. as for ellipses. that changes to green when the new element is within the specified tolerance. hyperbolas. This value must be greater than or equal to 2 along U. a red text is displayed if the tolerance is not respected.
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when the exact conversion cannot be performed. Select the curve to be approximated. Profiler & Optimizer
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Approximating/Segmenting Procedural Curves
In this task you will learn how to convert any curve. into a NUPBS (Non Uniform Polynomial B-Spline) curve. The maximum value allowed per segment is defined by the Max order field in the FreeStyle Settings and must be less than or equal to 16. 2. 1. and so forth. the converter Wizard is displayed allowing you to define the approximation tolerance. In this case: q when an exact conversion can be performed. Click the Converter Wizard icon . it must be greater than 4 included (when there are several segments). You need to set the values for the different options:
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Tolerance: that is the deviation tolerance from the initial curve. when the segmentation options are grayed (one segment only).

e. If Single is checked.
When one of these options is inactive. 3D conversion: to convert a curve on surface into a 3D curve 2. a text is displayed indicating what approximation needs to be performed:
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CV: the initial curve is not a NUPBS and needs to be approximated using the Converter Wizard parameters EXACT: the initial curve can be converted in exact mode (no parameter needs to be set) Seg: the initial curve already is a NUPBS
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Provided the Continuity icon
is active from the Dashboard. Orders. i. 2D conversion: to retain the 2D of a curve on surface
Depending on the type of the initial element. you are not in exact conversion mode). two buttons offer other capabilities: 1. Furthermore. the system automatically optimizes this option's parameters to comply with the other options' values. and at least one conversion
option is active (Tolerance. it is tangent. Two continuity types are available: tangent or curvature continuity. 3. Profiler & Optimizer
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Segmentation: that is the maximum allowed segments along the U direction. Click More>> to display more options:
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Check the Information option to display further information on the element:
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Max: the maximum deviation in relation to the initial element
. or Segmentation.FreeStyle Shaper. By default. a continuity constraint can be imposed identically on both curve end points. and you can change it either by using the contextual menu or by clicking the text in the geometry. a mono-segment curve is created.

4.
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Multi-selection of curves is available. Note that in this case. the initial element is duplicated. are: datum creation. minimum and maximum radius values are displayed in the Converter Wizard for information. The Priority check button indicates which of the Orders or Segmentation parameter is taking precedence over the other one. Profiler & Optimizer
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N: number of control points o: the curve order s: the number of segments in the curve
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r
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Check the Control Points option to display the curve's control points. and number of segments in the curve.
Furthermore. The curve modification is taken into account. continuity. and/or specified through the FreeStyle Settings. If selected in the geometry.
q
q
q
To convert a multi-cells curve.FreeStyle Shaper.
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Check the Auto Apply button to dynamically update the resulting curve. Use the Exact conversion mode (no parameter needs to be set) on a NUPBS element to display the number of control points.
. Click OK. and furtive display. curve order. keep original (depending on the selected element). the maximum deviation. You can mix the approximation of curves and surfaces. you might be selecting only one cell instead of the whole curve. Available capabilities from the Dashboard. select it from the specification tree.

or close it by clicking OK. or plane as reference element. set the extrusion direction and value. Create a surface from three points: click two points.FreeStyle Shaper. Create filling surfaces: select contiguous surface boundaries forming a closed contour. Profiler & Optimizer
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Creating and Managing Surfaces
This chapter deals with surface creation and management using the FreeStyle Shaper workbench. and define the angular limits of the revolution surface. set the deformation options. click a point. set the display options allowing the modifications of continuities and tensions. a rotation axis. Extrude a surface: select a curve. Create associative filling surfaces: select contiguous surface boundaries forming a closed contour. Rotate a surface: select a surface. Extrapolate a surface: select a surface boundary.
. Perform symmetry on geometry: select an element. using auto-detection capabilities. manipulate the coupling points defining the blend. move it close to geometry to detect another point to be used for projection or snap onto it. Manipulate surfaces: select a surface. drag the pointer over the surface and click another point still on the surface. move the surface along the compass axes. Edit a surface boundary: select a surface boundary and edit it using its control points. maximum orders. hold and glide on one of the compass' arc of circle Create planar patches: use the compass to define the creation plane. drag and drop the compass onto it. Use Manipulators: select a manipulator. Create a surface on an existing surface: select a surface. etc. pull on the control points and mesh lines in specific directions. line. drag and drop the compass onto it. the offset value and constraints to be taken into account when offsetting (deviation tolerance. Edit surfaces using control points: select a surface.
See also the FreeStyle Dashboard tools as they affect the curve creation and modification. then a point. click two points.). drag the pointer and click a third point. specify the extrapolation type and value. Create an ACA Fillet: click the icon and select two edges. Create a surface from four points: click at least three points on existing geometry and a fourth point. Offset surfaces: select a surface. select. Create blend surfaces: click an edge on two surfaces. specify the offset type (simple or variable). Create revolution surfaces: select a profile. or close it by clicking OK.

Create a Continuity Constraint: click the Continuity Constraint icon and select the elements to be connected. Match surfaces: select a surface edge and a boundary on another surface. set the smoothing weight and click Run.FreeStyle Shaper. and the resulting surface maximum orders and/or segments Copy geometric parameters: select the template curve and select the target curves. Concatenate surfaces: select a two-cell surface. Fragment surfaces: select a surface and specify the breaking options. Approximate/segment procedural surfaces: select a surface. Restore a surface: select the surface to be restored and click the icon.
. Multi-side matching: successively select a surface edge and its target curve on another surface. Profiler & Optimizer
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Smooth surfaces: select a surface. specify the extension type and value. specify the approximation tolerance. specify the matching parameters using manipulators on coupling and control points. and choose the disassembling mode. and use the contextual menu to set continuities or surface order. Extend a surface: select a surface boundary. and the contextual menu to set continuities and tensions.
Redefine surface limits: click the icon and select the part of the surface to be removed. and set the tolerance value. Disassemble elements: select a multi-cell element. or two separate surfaces. specify the matching parameters.

Drag and drop the compass over the surface you wish to move about. 4. The cursor shape changes to a cross. Open the Manipulate1.
1.FreeStyle Shaper. The compass now is displayed in green. Navigation tab to display the whole bounding box as shown below.CATPart document.
3. Click the Select icon
and select the surface you wish to move. Move the pointer over any bounding box boundary. not just the compass over the geometry.
Make sure you choose to display the bounding box using the Display manipulation bounding box option from the Tools -> Options -> General -> Display dialog box.
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Manipulating Surfaces Using the Compass
This task explains how to move and translate surfaces independently from any other element in the document using the compass. Point to the compass manipulation handle (the red square located on the privileged plane at the base of the compass).
5.
. Pull along a horizontal axis to slide the surface to the right or to the left. and drag the surface where you wish to move it.

Similarly you can pull along a vertical axis to move the surface up or down. The surface has moved to a new location.
For further details and general manipulation tasks refer to the Infrastructure User's Guide: Manipulating Viewpoints Using the Mouse and Compass and Manipulating Objects Using the Mouse and Compass.FreeStyle Shaper. Release the mouse-key. Profiler & Optimizer
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6.
7.
. The displacement distance is displayed as you move the surface around.

using the compass.
If you checked the option Display manipulation bounding box in the Navigation tab via the Tools > Options -> General -> Display menu item. a box will appear around the selected surface.
3.FreeStyle Shaper. The arc of circle is highlighted. Profiler & Optimizer
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Rotating a Surface Using the Compass
This task explains how to rotate surfaces independently from any other element in the document. Point to the compass manipulation handle (the red square located on the privileged plane at the base of the compass).CATPart document. 4. 1.
. Move the pointer over the arc of circle on the compass indicating the direction in which you want to
rotate the surface. 2. Select the surface you wish to move. Open the Manipulate1. The cursor shape changes to a cross. The compass now is displayed in green. Drag and drop the compass over the surface you wish to rotate.

whether using a trap or the Ctrl-click. The surface rotates within the plane indicated by the selected arc of circle. this has not changed anything to any other element present in the document. is available to rotate a set of elements. Profiler & Optimizer
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5. Release the mouse-key.
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The surface has rotated about an axis.
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. The surface is set to the new direction. However. Drag in the desired direction. 6.FreeStyle Shaper. Multi-selection.

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Creating Planar Surfaces
This task explains how to create planar patches. Make YZ the Privileged Plane: elements are created in the YZ plane c.
.CATPart document. that is planar surfaces.FreeStyle Shaper. However. By default the creation plane is the XY plane. The 3D compass is displayed in the document and looks like this: The solid planes of the 3D compass indicate in what plane any action is to be performed. 1. Open a new . Click the Planar Patch icon . Keep the default working mode. Make XZ the Privileged Plane: elements are created in the XZ plane b. Make Privileged Plane Most Visible: the plane in which elements are created is the plane seen most. you can right-click the compass to display other options: a.

the surface is created in the plane defined by the base.
If you call the function when a plane is selected. . 2. Profiler & Optimizer
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The surface is created in the current active plane as defined using the Current plane orientation toolbar containing the Flip to UV or XY WU or XZ icons.FreeStyle Shaper. the surface is created in the plane parallel to the compass base and passing through: r the origin of the model if the first point selected is in space
r
the first point selected on geometry
. An outline appears and evolves as you move the pointer in the main window.
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If the 3D compass is in the upper-right corner of the screen. Click anywhere in the window. Two values are displayed indicating the length and width of the patch. the surface is created in the selected plane otherwise it is created as described in the following cases. see Moving Objects Using the 3D Compass. Flip to VW or YZ or Flip to
To find out more about the compass. q If the 3D compass is in the model.

to edit the surface degree (in U and V) using the Orders dialog box just like you edited the dimensions.
. the planar patch is centered around the point corresponding to the initial click. this point corresponds to one corner or the patch. Profiler & Optimizer
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3. Using the Ctrl-key. and auto detection. simply click again when you have reached the adequate size. Right-click and choose Edit dimensions. and choose the Edit Orders menu item. If you do not explicitly enter the dimensions of the surface. right-click anywhere.
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Once the first point is defined.FreeStyle Shaper. The planar patch is created. by default. otherwise.
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Available capabilities from the Dashboard are: datum creation.

A line is displayed to show the direction. 1. Profiler & Optimizer
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Creating a Surface from Three Points
This task explains how to create surfaces by clicking three points in pre-existing geometry or space.CATPart document.FreeStyle Shaper. to define the first direction of the patch. or on already existing geometry. Successively click two points in space.
. Open a new . and a text indicates the length of the segment.
2. Click the 3-Point Patch icon in the Surface Creation toolbar.

the second length of this same patch being given by the distance between the first line and the normal projection from the pointer location onto the privileged plane containing the first point. and choose the Edit Dimensions menu item. Drag the pointer. Profiler & Optimizer
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3. to display the Dimensions dialog box that allows you to define exactly the second length of the
. A planar patch is pre-visualized and evolves as the pointer moves in space: the first two points making up the direction. You can also right-click.FreeStyle Shaper.

The surface is created in the current active plane as defined using the Current plane orientation toolbar containing the Flip to UV or XY WU or XZ icons. Click a third point to define the second direction of the patch as well as its area.
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Right-click and choose the Edit Orders menu item to edit the surface orders (U and V) at any time during the creation. . The planar patch is created. Use the Ctrl-key to create a patch symmetrically on each side of the segment defined by the first two points.FreeStyle Shaper.
. and auto detection. Flip to VW or YZ or Flip to
4.
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Available capabilities from the Dashboard are: datum creation. Profiler & Optimizer
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patch.

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Creating a Surface from Four Points
This task explains how to create surfaces by clicking four points in pre-existing geometry and space. Open the FourPointsPatch1.CATPart document. 1. Click the 4-Point Patch icon in the Surface Creation toolbar.

2. Click one of the curves. You can click anywhere on any curve, at the intersection of curves, or on any other element.

3. Successively click two other points on the pre-existing geometry. An outline is previewed, representing the surface as it is defined.

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4. Click anywhere in the document to create the last point used in the surface definition. If you click in space, the patch is a planar patch that belongs to the plane defined by the first three points. If you click the fourth point on existing geometry, the resulting surface will not necessarily be planar.

5. Once all four points have been clicked, the corresponding surface is automatically created.

q

Right-click and choose the Edit Orders menu item to edit the surface orders (U and V) at any time during the creation. Available capabilities from the Dashboard are: datum creation, and auto detection.

q

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Creating a Surface on an Existing Surface
This task explains how to create a surface on an existing surface. The newly created surface will lie on the initial one.

Open the SurfOnSurf1.CATPart document. 1. Select an existing surface. 2. Click the Geometry Extraction icon 3. Click on the surface, where you would like a corner of the new surface to be located. If you press the Ctrl-key while clicking, the surface is created symmetrically in relation to the initial surface center. .

4. Drag to generate a rubberband matching the new surface. 5. Click once you are satisfied with the new surface as visualized.

6. A surface is created lying exactly on the initial surface:

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As opposed to the creation of planar patches, you cannot define the surface orders (U and V) prior to or while creating the surface. The resulting surface orders are identical to those of the initial surface. However, these values can later be edited (see Editing Surfaces Using Control Points). These surfaces, as any other surfaces, can be edited using the control points. If you move the pointer to the edge of the initial surface, the new one will automatically snap on the initial boundary. Similarly, you can create curves on an already existing curve. Using the Ctrl-key will then create a curve symmetrically in relation to the initial curve center. See Creating Curves on Surfaces to find how to use the remote auto detection capability.

q

q

q

q

Only the datum creation capability is available from the Dashboard.

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Extruding Surfaces
In this task you will learn how to create a surface by extrusion from a curve. This can be any type of curve, such as planar curves, 3D curves, surface edges, or curves on surfaces. Open the Extrude1.CATPart document. 1. Click the Extrude Surface icon .

2. Select the curve from which you want to extrude a surface. A manipulator is also displayed on the curve, oriented according to the 3D compass. The Extrude Options dialog box is displayed: q the Normal to the curve icon is the default icon and indicates the direction orthogonal to the curve plane
q

the Compass direction icon enables you to manipulate elements using the 3D compass the Length field indicates the extrusion length the Display corners check button, allows the visualization of manipulators at the curve extremities

q

q

All the parameters entered in this dialog box are retained when the box is closed. 3. Click the manipulator on the curve and drag the pointer to extrude the surface in the given direction.

Capabilities are available from the contextual menu when right-clicking the manipulator. When you press the Ctrl-key while dragging the pointer, you can perform a symmetry.

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The previewed extruded surface is dynamically displayed as you drag. The segment number and the degree of the resulting surface are displayed:
q

a full line indicates the segment limit a dashed line indicates the surface order

q

You can move back and forth between the compass and the surface to define the orientation after having extruded the surface, as long as you have not performed the final step.

4. Click OK to create the surface.

q

When the selected curve is not a 3D NUPBS (Non Uniform Polynomial B-Spline) curve, the Cv text is displayed. Right-click the Cv text and choose the Edit contextual menu to access the Converter Wizard allowing you to control the curve (order and segment number) on which the new surface is based.

q

Check the Furtive Display icon

to

visualize the initial curve control points as you are extruding it.
q

You can select the edges of the surface to extrude either by: r clicking on them in the 3D geometry
r

using the selection trap (all the edges will be selected) clicking the surface in the specification tree (all the edges will be selected)

r

q

Available capabilities from the Dashboard are: datum creation, auto detection (Snap On Vertex and Snap On Cpt options only), attenuation, and furtive display.

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Creating Revolution Surfaces
This task shows how to create a surface by revolving a planar profile about an axis. Open the Revolution1.CATPart document.

1. Click the Revolve icon

.

The Revolution Surface Definition dialog box appears.

2. Select the Profile and a line indicating the desired Revolution axis. 3. Enter angle values or use the graphic manipulators to define the angular limits of the revolution surface.

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4. Click OK to create the surface. The surface (identified as Revolute.xxx) is added to the specification tree.

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There must be no intersection between the axis and the profile. However, if the result is topologically consistent, the surface will still be created. If the profile is a sketch containing an axis, the latter is selected by default as the revolution axis. You can select another revolution axis simply by selecting a new line.

q

Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

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Offsetting Surfaces

This task explains how to create an offset surface, based on an existing surface. Open the Offset1.CATPart document. 1. Select a surface, or a set of surfaces.

2. Click the Offset icon

.

The offset surface is automatically visualized as a meshed surface.

3. Choose the options you wish from the Offset Surface dialog box:

q

the offset type: a simple offset creates a surface which points are all at the same distance from the initial surface, whereas a variable offset lets you set the offset distance at each corner point of the surface. the limits, that is constraints to be taken into account when computing the offset surface. You can specify whether it should comply with a given tolerance, or it should have a maximum order in U and V. The resulting surface will lie within these constraints. Display, that is the elements to be displayed on the geometry.

q

q

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When you click the More... button: the type of information to be displayed on the offset surface before it actually is created. This information is useful to let you fine-tune the offset specifications. q Offset values: the distance between any point of the initial surface and the resulting surface.
q

Normals: identifying the direction of the initial surface. Click on the arrow to invert the offset. Order: the order value in U and V Tolerance: the exact tolerance deviation Corners: displays or hides the manipulators at the four corner points (only in Simple mode) to make Snap on Geometry possible. When you are in Variable mode, the Corners option is checked: if you pull the central manipulator, all manipulators are temporarily linked to each other, basically they have the same behavior as regular control points.

q

q

q

4. By default the Edit dialog box is displayed. If not, right-click the offset value box on the surface to display it, and enter the offset value.

5. Click Close to validate the offset value. You can also move the pointer over one of the corner points, and directly pull on the displayed manipulators. The offset value is dynamically modified.

You can also select a point either in the 3D or in the specification tree to impose the offset value. The value will be set as well as the distance corresponding to the normal projection of the input point onto the surfaces.

Offset values are displayed at each corner of the surface.
Right-click another offset value and using the Edit dialog box. no selection is possible and a message error is issued. This means that the maximum order number of the offset surface will not exceed the initial surface order number plus the indicated value.
e. c. You can also create variable offset: a.
Click OK in the Offset Surface dialog box. Here we modified two values from 15 to 40. b.
. The offset surface is created. change this value. Move the pointer over a corner point and drag it in the desired direction to dynamically modify the value. Profiler & Optimizer
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If no projection is possible.
d. You can modify the delta in order. Click Variable in the Offset Surface dialog box.FreeStyle Shaper.

. keep original. auto detection.FreeStyle Shaper. check the Normals option from the Offset Surface dialog box and right-click arrows: a contextual menu displays on each arrow and enables you to Reverse or Adjust all. and furtive display. Nevertheless. Profiler & Optimizer
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q
The same method applies when offsetting a set of surfaces. even though the pre-visualization presents the initial (not relimited surface):
q
If the offset value is superior to the maximum value. attenuation. Capabilities are available from: q the contextual menu when right-clicking the manipulator
q
the Dashboard: datum creation. the result is a relimited surface.
Multi-selection of surfaces is available. an error message is issued. As all surfaces may not present the same orientation. you can create the offset.
q
If the offset is performed on a surface relimited using the break command.

and the Curvature option active. Select a surface boundary.
Similarly. The extrapolated surface is created. The extrapolation is pre-visualized and dynamically evolves as you modify the extension length. Here are two views of the extrapolated surface. Open the Extend1. that is add an extra surface to the initial one while taking continuity constraints into account. A manipulator is displayed.
q
Curvature: the surface is extrapolated by the specified value. the surface is extrapolated according its initial curvature:
. and of a given distance (G1 continuity).
The Extrapolation dialog box is displayed. illustrating the tangency constraint on the selected edge. Profiler & Optimizer
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Extrapolating Surfaces
In this task you will learn how to extrapolate a surface. You could just as well enter the value directly in the Length field.FreeStyle Shaper.
4. complying with the surface curvature (G2 continuity). Two options are available: q Tangential: the surface is extended along the tangent to the surface on the selected boundary.CATPart document. No manipulator is displayed. 2. Click OK. if an edge is selected. 1. Click the Styling Extrapolate icon .
3. Click Tangential and pull on the manipulator till you reach 60 in the Length field of the Extrapolation dialog box.

there may be no possible result in some cases. before clicking the Extrapolate icon . you need to select these.
q
The curvilinear length between the middle of the selected original surface edge and the middle of the extended surface is displayed. Since you chose this constraint.
r
q
when the Exact option is not checked. the extrapolation is computed according to the geometric mode. r when the Exact option is checked. Only the datum creation capability is available from the Dashboard. computation is analytical and the resulting surface presents the same degree as the initial surface. using the Ctrl-key. check the Exact option if you want to switch to the exact mode.
q
. Profiler & Optimizer
q
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With Curvature option With Tangential option To extrapolate a set of surface boundaries. capabilities are available from the contextual menu when right-clicking a control point. The figures below show a surface extrapolated when Exact mode is checked and unchecked.FreeStyle Shaper.
q
Exact mode not checked Exact mode checked Using the Tangential option. Whether in Tangential or Curvature mode.

Profiler & Optimizer
Creating Blend Surfaces
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This task explains how to create a blend surface between two pre-existing surfaces.FreeStyle Shaper. the pointer is over the surface when selecting the edge)
. in Approximated mode. the blend surface presents a point. based on the selected surfaces' control points. then. You can select edges either from outside the surface (i. 1. Moreover. and the Blend Surface dialog box is displayed. depending on the geometry configuration.
q
When in P1 mode.
The blend surface is previewed.e. In this case. the pointer points towards the surface) or from within the surface (i. it is best to use the Proportional continuity. that allows the creation of the blended surface while taking the tangency continuity into account. if not possible. twisted surfaces may be generated. tangency and curvature continuity with the initial surfaces. only the Auto mode is available. trying first to create the blend surface in Analytic mode. Information on the blend surface is displayed in the Blend Surface dialog box:
q
the blending type used (especially useful when working in Auto mode) the number of patches making up the surface the order of the blend surface along U and V
q
q
2. Move the pointer over one of the surfaces and click one of its edges.CATPart document. then check the continuities if needed. When in analytic mode and Tangency continuity. Auto: the system optimizes the computation mode.
Three modes are available to create blend surfaces: q Analytic: when the selected surface edges are isoparametric curves.
q
Approximated: regardless of the type of the selected surface edges. Open the BlendSurface1. the blend surface is created according to an approximation between the initial surfaces. Click the FreeStyle Blend Surface icon . the blend surface is computed in exact mode.e.

normal) at each point of their connection. From the Dashboard. Proportional and Curvature. click on the Continuity icon and right-click onto the identifier to edit the continuity constraint on the boundary of the blend surface and the selected surfaces. surfaces share a common tangent plane (i. appears. but the longitudinal variation from one point to the other is smoother.
In case the selected edge relies on more than one support. Change both continuities to Tangent.e. click the Tensions icon .
4. Curvature: the surfaces share a common curvature and tangent plane at each point of their connection 6. the Please refer to Selecting a Support for further information.FreeStyle Shaper. normal) at each point of their connection Proportional: similarly to the Tangent option. Click the edge of the second surface.e.
. there is no gap between the surfaces
q
Tangent: the surfaces share a common tangent plane (i. as the system automatically re-distributes the control point location on the blend surface This mode is automatically set for both limits of the blend surface.
q
q
The tension values are displayed on the element along with a green segment representing the direction and limits of the blend surface tangent at its middle-points.
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The
tag informs you that there is only one surface to be selected. Right-click a limit point and choose one of the options from the contextual menu. q Point: the surfaces share each point of their common boundary. Tangent.
5.e. The blend surface is automatically previewed. Profiler & Optimizer
3. i. Still from the dashboard.
Available continuity types are: Point. using the contextual menu. You can modify the tension values by sliding the green triangle along the direction.

Right-click on the top boundary tension identifier and choose Invert direction. This homogenization is only possible with an approximated blend surface.
. providing they are built on the same supports. Profiler & Optimizer
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7. you can modify the local tangent and curvature parameters. If you move the coupling points onto the edges of the support surface.
q
In the case of an approximated blend type. You can modify the tangency between the free edges and the edges of the support surface by clicking either Tangent or Normal.FreeStyle Shaper. only the normal direction is kept for the free edges of the blend
q
Tensions are now homogenized between blend surfaces and blend curves. so that the borders of a blend surface have the same shape as the blend curves.

Click OK in the Blend Surface dialog box to create the blend surface.
to deactivate the tensions.
You can edit the contact points by right-clicking any of them to display the contextual menu and choosing the Edit item. and click the Contact
Manipulators are displayed on the connection. in percentage of the total boundary. To the right is the resulting blend without the Project end points option.FreeStyle Shaper. control points of the created element are displayed. if selected first.
9.
The Project end points option allows linear projection of the smaller edge. The Tuner dialog box opens to let you key in a new value. onto the other surface as shown to the left. Invert the top tension to come back to the initial surface.
. thus allowing to immediately analyze its connection to the other surfaces. allowing you to interactively define the blend limits by simply sliding them along the boundaries. click Points icon .
If you click on the Furtive Display icon
from the dashboard. for example. It remains selected. Profiler & Optimizer
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8.

tensions. Modifying the continuity may enable the blend creation. and/or specified through the FreeStyle Settings. contact points. continuity. are: datum creation. Available capabilities from the Dashboard.
. Profiler & Optimizer
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Should there be a twist between the two surfaces. and furtive display. the blend surface is not created.FreeStyle Shaper.

FreeStyle Shaper.
. Open the ACAFillet. Profiler & Optimizer
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Creating an ACA Fillet
This task explains how to create an ACA fillet surface between two given surfaces. Two vectors and the continuity symbol appears (G2). Select the two edges where you want to create the fillet.
2.CATPart document
1. The Fillet dialog box is displayed. Click the Fillet icon .

When you activate minimum radius.
. Alternatively. you can change the value using the up and down arrows in the Minimum Radius . Profiler & Optimizer
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3. Click Apply create the fillet. a new vector appears enabling you to change the minimum radius in the middle of the fillet.FreeStyle Shaper.
4.

. variable fillet is not possible Options r Extrapolate . (G0 . Profiler & Optimizer
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The dialog box displays several options helping you to create the fillet: q Continuity : Quality of continuity between fillet and reference surfaces. please refer to the CATIA Automotive Class A documentation.FreeStyle Shaper.Face trimming of reference surfaces on fillet boundaries Variable .Instead of the radius. If no common edge is detected.Activates variable radius (only possible if edge tolerance is met) Chordal Fillet (only for Variable off) . Trace curves will be computed in dependency of G2
q
Arc Type (only for G1) r Blend : Creates a blend surface between the traces
r
Approx : Creates a circular bezier approximation Exact : Creates a rational surface with true circular sections
r
q
Parameter : Different options for parameterization of the result and fillet surface r Default : Internal computed best filling parameterization
r
Patch 1 : Parameterization is taken from the 1st patch Patch 2 : Parameterization is taken from the 2nd patch Average : Average of parameterization from patch 1 and patch 2 is taken Blend : Traces have parameterization of their correspondent surface
r
r
r
q
Edge Tolerance : Tolerance for common edge detection.Fillet surface also on extrapolation of reference surfaces
r
q
Trim . the chord length of the cross-sections defines the fillet
r
r
For further information.G2)
q
Segments/Order : Order of the fillet surface in direction of common edges Radius : Fillet radius Minimum Radius : Minimum radius in the middle of the fillet (optional) r Relative : Minimum radius is relative the minimal variable radius
r
q
q
True Minimum (only for G2) : Minimum radius is controlled.

4. the filling surfaces are created. 1. depending on the geometry configuration.
3. Tangent continuity is available only when filling a closed contour. Select the boundary of the first surface.CATPart document. These elements must be contiguous in only one point.
Once you have selected the last boundary contiguous to the first selected surface.FreeStyle Shaper. Select the boundary of an adjacent surface. The elements can be either curves or any surface type element.
If you checked the Continuities option from the Dashboard (P2) or the FreeStyle Settings. Click the Fill icon . You can fill the space between three or more elements (up to nine). You can choose from Point or Tangent continuity.
The Fill Options dialog box is displayed allowing you to define the Deformation direction (P2 only). still going from one surface to its direct neighbor. Select the boundary of all other surfaces.
. Profiler & Optimizer
Creating Filling Surfaces
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In this task you will learn how to fill the space between three surfaces. This will let you deform the resulting filling surfaces according to the Compass Direction or Normal to the Surface Direction.
2. the corresponding information is displayed on the surfaces:
5. Right-click the displayed text to edit the continuities. Open the Fill1.

The center point is not displayed if only one filling surface is created or when four filling surfaces are generated.
. To this end. simply select these curves or surface boundaries. A temporary blend curve is created to close the contour when you click Apply. To do this. allowing the system to compute the filling surfaces. and the filling surface created accordingly. you can fill three or more open-sided contours when composed of surface boundaries only.FreeStyle Shaper. only the Point continuity is available on the curve. Furthermore.
7. set continuities are retained.
You can also fill the space between two intersecting curves.
While deforming. forming an open angle. You can fill the space between different types of elements. Use the manipulators at the center point (P2 only) to deform the generated surfaces. Graphic tab. The deformation depends on the chosen icon: Normal to the Surface Direction. the intersections between the selected edges on the surfaces and the blend limits are automatically detected. Profiler & Optimizer
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6. select a curve.
Capabilities are available from the contextual menu when rightclicking the manipulator. then click Apply in the Fill Option dialog box.
q
You can use the graphic properties to modify the colors of the filling surfaces to better identify them. In this case. and call the Properties dialog box. select each surface either in the geometry or in the specification tree. For example. or according to the Compass Direction.
q
Similarly. The system automatically creates temporary curves matching the selected ones to close a contour before filling it. or surfaces. Click OK to create the filling surfaces. two surfaces supporting a blend surface and the blend itself. and modify the Fill color.

If four edges have been selected. are: datum creation. as many surfaces are created as selected edges.01 mm) is identified for correction purposes. that exceeds the set tolerance (0. A text is displayed. and/or specified through the FreeStyle Settings.01 mm. and the fill cannot be performed. continuities and furtive display.FreeStyle Shaper. If the gap is smaller than 0. the fill is automatically performed complying with the tolerance all around the selected edges. Profiler & Optimizer
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q
Make sure you select contiguous surface boundaries. indicating the gap value. temporary analysis. auto detection (Snap On Edge option only). Available capabilities from the Dashboard. attenuation. five or more edges (up to nine) have been selected.
q
q
q
. A gap between two selected boundaries. if three. a mono-patch surface is created. especially when filling the space between more than three surfaces. Do not select boundaries randomly. However.

FreeStyle Shaper.CATPart document.
r
If there are four elements. The elements can be either curves (only one intersection between the curves is allowed) or any surface type element. Profiler & Optimizer
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Creating Associative Filling Surfaces
In this task you will learn how to fill the space between three or more surfaces. These elements must be contiguous in only one point. five or more elements. depending on the number of elements. one surface will be created with supporting edges as borders If there are three. several surfaces (four-side surfaces) with a barycenter point will be created: there will be as many surfaces as there are continuity changes:
. You can fill the space between three or more elements (up to nine). 1. Choose the Fill Type:
q
Analytic: one or more filling surfaces will be created. Click the FreeStyle Fill icon . The Fill dialog box displays:
2. Open the Fill2. two cases can occur:
r
1.

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2. one or n surface(s) (four-side surfaces) will be created if a continuous continuity between the elements is respected. we chose the Auto type.
q
Power: one filling surface is created. Select the boundary of the first surface.
.FreeStyle Shaper. All continuity types are available using the contextual menu Auto: the best orders and number of patches will be chosen by the application depending on the inputs
q
In our example.
3.

If you checked the Continuities option from the Dashboard (P2) or the FreeStyle Settings.
.FreeStyle Shaper. Profiler & Optimizer
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4. number of patches.
Information on existing gaps between supporting edges is displayed in the 3D geometry.
The Information frame informs the user about the resulting fill: type.
5. the filling surface is created. and the U/V order. the corresponding information is displayed on the surface. Once you have selected the last boundary contiguous to the first selected surface. Select the boundary of an adjacent surface. Here the most appropriate type for this fill is the Analytic type. Select the boundary of all other surfaces. The maximum gap value allowed is 0. appears.
The
tag informs you that there is only one surface to be selected. the Please refer to Selecting a Support for further information. still going from one surface to its direct neighbor.
In case the selected surface relies on more than one support.1mm.

the more precise the created fill surface is. You can specify whether it should comply with a given tolerance. The resulting surface will lie within these constraints.
. Please refer to the Customizing section.
r
The Maximum Tolerance and Order are defined in Tools -> Options -> Shape > FreeStyle.
7. that is constraints to be taken into account when computing the fill surface. Click More>> to display further options:
q
Limits.1.FreeStyle Shaper. or it should have a maximum order in U and V. r U/V Orders: number of control points by patch The minimum orders 2 / 2 for all fill types
r
U/V Patches Tolerance: the maximum tolerance is 0. Profiler & Optimizer
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6. The smaller the tolerance is. Check the Furtive Display option from the Dashboard (P2) to display the control points and visualize the number of orders.

Tangent continuity is available only when filling a closed contour.FreeStyle Shaper. Tangent or Curvature continuity.
9. five.1 mm. if you create a new fill. Profiler & Optimizer
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If you create a fill then you decrease the order value in Tools -> Options -> Shape -> FreeStyle.001 mm and 0. the maximum value would still be 0. 8. The tolerance value is comprised between 0. depending on the geometry configuration. or more input elements. until it reaches the value defined in Tools -> Options -> Shape -> FreeStyle. You can choose from Point. the new order value will be set as the maximum value.
. Right-click the displayed text to edit and modify the continuities. However.1 mm. Options in the Limits frame are grayed in the case of an Analytic type with three. May you define a higher value. the maximum order value will be the one defined in Tools -> Options -> Shape > FreeStyle. Click OK to create the filling surfaces. Nevertheless. if you edit the fill and decrease its order value directly in the Fill the dialog box. the created fill will keep the former value.

set continuities are retained. Capabilities are available from the contextual menu when right-clicking the manipulator. It has also the possibility to snap on any particular point. While deforming. The deformation depends on the chosen icon: Normal to the Surface Direction.FreeStyle Shaper. This point translator can be moved along a normal to resulting fill or on one of the compass direction. Profiler & Optimizer
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The Constraint option you to define the Deformation direction (P2 only). The deformation direction after fill creation is managed by the center point frame and the point translator into 3D model.
. Use the manipulators at the center point (the barycenter point) to deform the generated surfaces. The Constraint option is only available with the Analytic type. or according to the Compass Direction. This will let you deform the resulting filling surfaces according to the Compass Direction or Normal to the Surface Direction.

Select a point. 1. Select the Element to be transformed by symmetry.
.
The figure below illustrates the resulting symmetry when the point is used as reference element.FreeStyle Shaper.
2.
The figure below illustrates the resulting symmetry when the line is used as reference element. and Profiler.
The Symmetry Definition dialog box appears as well as the Tools Palette.CATPart document. Click the Symmetry icon . line or plane as Reference element. 3. Optimizer. Profiler & Optimizer
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Performing a Symmetry on Geometry
This functionality is P2 for FreeStyle Shaper. This task shows you how to transform geometry by means of a symmetry operation. Open the Transform1.

The element (identified as Symmetry. This switch only concerns volumes since the transformation of a surface can only be a surface.xxx) is added to the specification tree.FreeStyle Shaper. Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option. To have further information about volumes.xxx in the specification tree. you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. however the associated icon is the axis system's .
q
Use the Hide/Show initial element button to hide or show the original element for the translation. Click OK to create the symmetrical element. Profiler & Optimizer
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4. refer to the Selecting using a Filter chapter in the CATIA Infrastructure User's Guide. Note that the switch between surface and volume is greyed out when editing the feature. Thus in case of multi-selection of volumes and surfaces. please refer to the corresponding chapter. You can select an axis system as the Element to be transformed. the switch only affect volumes. The following capabilities are available: Stacking Commands and Selecting Using Multi-Output. The element is identified as Symmetry. providing it was previously created.
. To select a sub-element.
q
q
Note that the selection of the feature prevails over the selection of the sub-element. For further information.

Open the EditControlPoints1. the Converter Wizard will be automatically displayed when the surface cannot be exactly converted. it will modify the compass orientation. However. control points and mesh lines are displayed. Click the Control Points icon
. Profiler & Optimizer
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Editing Surfaces Using Control Points
This task explains how to modify a surface using control points and mesh lines. This allows you to control the conversion tolerance. If you select a surface that has been created outside the FreeStyle workbench.
2. Therefore if you select a plane or a line. the conversion is done automatically and an information message is issued.
As soon as you clicked the icon.
The 3D compass is displayed showing the privileged plane in which you are working when you are manipulating the surface.
It will be duplicated if the Keep Original icon is active in the FreeStyle Dashboard. the Converter Wizard is not displayed.
.CATPart document.FreeStyle Shaper. when a surface can be exactly converted. and the surface is not based on a NUPBS (Non-Uniform Polynomial B-Spline).
Planes and lines are used to quickly orientate the compass in the control points command. 1. Select the surface. They are used to manually pull on the surface so as to deform it.

Stretch selected points You cannot specify a Support. In P1 mode.
4. Move selected points identically 2. They represent the directions in which you can perform a deformation. Manipulators automatically appear. The surface follows the shape indicated by the mesh line or
. Move the pointer onto one of the control points or mesh lines. you can modify curves according to two laws only: 1. Profiler & Optimizer
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The Control Points dialog box is displayed: Use it to define the type of operation to be performed on the control points. choose the Translation along the normal to the surface and Bell law options.
q
For further information on supports and laws.
q
Support defines the type of translation to be applied Law defines the type of deformation that is to be applied when several control points have been selected.
3. refer to How to Use the Support and Law Options? Here. Pull on the arrow matching the direction in which you want to deform the surface.FreeStyle Shaper.

. in the Control Points dialog box.FreeStyle Shaper. 5. or select a set of points using the Ctrl-key or Shift-key while clicking (multi-selection capabilities).
By default all control points and mesh lines are selected. Click More.
q
Using the Harmonize icon
you smoothly propagate the control points organization
over the surface. You can activate other support and law options and continue deforming the surface. It is especially useful when the boundary mesh lines have been constrained within a given plane for example. Further modification options are available:
q
Selecting all control points or de-selecting them all at a time without clicking in the geometry. Profiler & Optimizer
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control point. The same applies to mesh lines. Click a specific point to deform the surface at this point only...

The continuity type affects how the surface border is evolving when the whole surface is modified. use the Dashboard's the Continuity Orders and U. You can edit these by rightclicking the displayed text.FreeStyle Shaper. some modifications may no longer be possible Dynamic display of the initial surface and of the delta as you pull on the control points. Tangent and Curvature.e.
q
The initial surface is represented by black solid lines (external edges) and dotted lines (inner isoparametric curves). Available continuity types are: Free. Profiler & Optimizer
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Freezing of directions or of the selected points (no other can be selected) and the modification can be performed only according to the allowed directions. Point.
To display the order number and continuity type directly on the surface.
q
Smoothing (refer to Smoothing Surfaces). A warning message can be displayed on the geometry when the chosen continuity and the chosen Support and Law do not
. or continuity type. V icons (P2) or the
specified settings (using the Tools -> Options -> Shape -> FreeStyle menu) (P1). The maximum deviation is given for information. and choosing a new order number. i.

continuity constraints are not detected. and are green when deselected.
When selecting several surfaces. if a continuity constraint exists. or mesh line to deform the surface at this element only.FreeStyle Shaper.
If the Manual Update mode is activated in Tools -> Options > Part Infrastructure -> General tab. the continuity tag displayed is set by default to the same continuity imposed by the constraint. Profiler & Optimizer
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comply. By default.
.
6. selected points are displayed in red. The surface is modified. Click OK in the Control Points dialog box to validate the modifications.
q
Click any specific point.

It lets you define the ratio between the mouse displacement and the actual displacement of the manipulator. Profiler & Optimizer
q
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Deformation can also be done using the Tuner dialog box displayed using the Edit contextual commands on control points or mesh lines.. You cannot move unselected points unless no point is selected.
q
To snap a point onto external geometry. without having to click the geometry..
q
q
The following options are available in P2 mode only:
q
Further modification options are available from the More.
. This attenuation factor is saved in the CATIA settings. use the auto detection capability from the Dashboard. In P2 mode. Once the value has been defined in the Tuner dialog box. use the attenuation capability from the Dashboard. button of the Control Points dialog box: r Freezing of the selected points (no other can be selected) and of the Support option
r
Dynamic display of the initial curve and of the delta as you pull on the control points Global selection/de-selection of control points using the Select All Select All and De-
r
icons as shortcuts to select/release all control points of the selected
elements. choose the Inflections checkbox.FreeStyle Shaper. press and hold the Shift key then click one of the manipulator's arrow to move the selected control point by the defined step value. the following manipulation options are available: q To fine-tune the manipulators.. With this dialog box you can: r specify the exact position of the control point in space
r
define a step value by which a control point/mesh line moves (Step field). To perform a quick analysis of the mesh line inflection.
Use the Manipulators (arrows) to modify the surface.

and depending on the geometry. Select a mesh line or a subset or control points (you can also select all points but in this case the whole surface is projected according to the compass) 3. Select All.
q
The Enable local plane detection icon allows
you to find whether certain control points and mesh lines are aligned within a specific plane. when several element have been selected. Bring the 3D compass onto the surface 2. applies the chosen capability on this element only. a given all the selected elements will be affected. Click the Projection icon . text are displayed along U and V indicating where the detection is active. and De-Select All capabilities are also available on the contextual menu displayed when right-clicking a control point.
. or not. and not on the whole selection. the planar organization of control points in one direction. Profiler & Optimizer
q
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The Freeze. However.
q
Projection: Use this capability to project selected points according to the local 3D compass either in the current plane or according to the normal to the current plane:
1.
Right-click these texts to choose to retain. with the following capabilities: r Project on the plane
r
Project on the normal Harmonize
r
Note that using the contextual menu on an element.FreeStyle Shaper. if you apply the same capability from the Control Points dialog box.
In this case.

and click one of the following icons:
-
: the points are
projected along the compass plane
-
: the points are
projected along the normal to the current plane.
.FreeStyle Shaper. Profiler & Optimizer
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q
Select a mesh line and the compass plane.

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q
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Click the Symmetry icon to perform a symmetrical modification in relation to the current plane. by selecting either: s a local plane. or to define a new plane as the current plane (by clicking Cancel first.
q
Use the F6 key to "quickly" orientate the compass : r along an axis.
s
a mesh line. See Managing the Compass.
You can choose to use the current plane (by clicking OK in the dialog box). then creating a new plane). you can modify its location using the manipulator. or two control points
s
r
in a plane. by selecting either: s an existing plane. Use the F5 key to display the quick compass orientation toolbar and move the manipulators into a different plane of the compass.
. prior to confirming its use in the dialog box. the control points are deactivated. or three control points
s
When you click this key. If you choose the current plane.FreeStyle Shaper.
s
two mesh lines.

continuities and orders
q
q
The Harmonize and Local Detection capabilities are only available with the FreeStyle Optimizer product. from the Dashboard. attenuation. are: datum creation. keep original.
. Profiler & Optimizer
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q
Press both F6 and Control keys to create either a Mean Plane or a 3 Point Plane plane using control points in order to project them: r Mean Plane: select a mesh line
r
3 Point Plane: select a point. the two extreme points are automatically defined
Capabilities are available:
q
from the contextual menu when right-clicking a control point. auto detection. specified through the FreeStyle Settings.FreeStyle Shaper.

.
Open the CurveOnSurface2.
4. Select the surface boundary you wish to edit. Profiler & Optimizer
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Editing a Surface Boundary
This task explains how to modify a surface boundary as created in Creating Free Form Curves on Surfaces using its control points.
By default all control points are selected. Click OK in the Control Points dialog box.
Control points and lines are displayed along that boundary.CATPart document. Modify the boundary pulling on its control points or the mesh line.FreeStyle Shaper. 3. Click the Control Points icon
. 1. The boundary is modified. Click a specific point to deform the boundary at this point only.
2. or select a set of points using the Ctrl-key or Shift-key while clicking (multiselection capabilities).

are: datum creation. Profiler & Optimizer
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Only the boundary and its control points are modified. Any other boundary of the surface is not affected by these modifications.
.FreeStyle Shaper. from the Dashboard. auto detection. specified through the FreeStyle Settings. continuities and orders.
Capabilities are available: from the contextual menu when right-clicking a control point. attenuation. See also Editing Curves Using Control Points.

Using a point for a projection An alternative method consists in selecting the first (yellow) surface first. the first surface's control points turn gray and remain frozen.
Resulting deformed surface
.
3. and the point on the second surface is identified by a dotted circle. the Use this point text is displayed.
5.FreeStyle Shaper. onto the support as defined in the dialog box. clicking the Control points icon. Profiler & Optimizer
Using Manipulators
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When working with the FreeStyle workbench a number of manipulators are displayed. respectively. 1. When using the Control Points capability ( icon) the points are constrained according to the chosen Support and Law options (see Editing Curves Using Control Points and Editing Surfaces Using Control Points). On the blue surface select only one control point. This projected location is identified by a red circle connected to the detected point on the second surface by a dotted line. This is especially useful when using the Move selected points identically option from the Control Points dialog box.CATPart document. allowing you to modify the shape of curves and surfaces. the selected point on the blue surface is located at the orthogonal projection to the point detected on the second surface. These manipulators are displayed as green dots with two to four arrows. Select both surfaces.
4. 2. and in P1 mode. All other points turn to green and the selected point is highlighted. Click the Snap on Ctrl points in the Dashboard. Move this point close to the other surface. then selecting the second (blue) surface. Click the Control Points icon . If you release the mouse button then. depending on whether they are constrained in a given plane or allowed to move freely in space. In this case. As the pointer nears a control point onto the other surface. Open the Manipulate2.

the selected point is moved exactly to the location of the point on the second surface identified as the point to be snapped to. when matching the two surfaces. as the manipulators are constrained on the surface's edge:
Using the Shift key to use a point
Using the Shift + Ctrl keys to snap onto a point
Resulting matched surface
Capabilities are also available from the contextual menu when rightclicking a control point. Profiler & Optimizer
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6. and depending on the geometry. as if they were merged. with the following capabilities:
. Press the Control key: the text changes to Snap on this point. For example. Using a point or snapping onto it is identical. and snap on points.
Snapping onto a point
Resulting deformed surface
The snap onto a point is possible only when the selected point is not constrained onto a specific element. In this case.FreeStyle Shaper. along the other surface's edges. the manipulators are only allowed to move.

when they are not constrained within a given direction. h. i. if you apply the same capability from the Control Points dialog box. f. Keep this point: allows you to keep the current point at its location. Freeze: enables to set control points inactive according to the defined constraint.define a step value by which a control point/mesh line moves (Step field). Profiler & Optimizer
a. Edit: the Tuner dialog box is displayed. When no auto-detection mode is active. or not. a given all the selected elements will be affected. press and hold the Shift key then click one of the manipulator's arrow to move the selected control point by the defined step value.
q
q
Snapping is available in P2 mode only. to another element. applies the chosen capability on this element only.FreeStyle Shaper. and not on the whole selection. e.
. Use the Shift key to activate/deactivate temporarily the auto-detection capability on the point you are currently trying to snap. See Managing the Compass. Use the F5 key to move the manipulators into a different plane of the compass. letting you
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-specify the exact position of the control point in space .
b. Keep all points: allows you to keep all the control points All the points appear in the specification tree d.xxx appears in the specification tree c. Once the value has been defined in the Tuner dialog box. g. Project on the plane Project on the normal Harmonize Select All: enables to select all control points De-Select All: enables to de-select all control points
Note that using the contextual menu on an element. However. when several element have been selected. A Point. manipulators will be snapped onto corners or onto another manipulator.

5. and smoothing is performed on these points only. Click the Control Points icon
. 4. You can choose at which point. Define the smooth weight. the surface should be smoothed. press and hold down the Ctrl-key. The surface is smoothed according to the value. Still maintaining the Shift key down. 1. click another point of the curve. Profiler & Optimizer
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Smoothing Surfaces
In this task you will learn how to smooth a surface. Select the surface to be smoothed. then move on to the other points to be selected.
3.
2. All points selected between the two selected points are selected as well. and the surface is smoothed in this area only.
You do not need to select the whole surface. Once you are satisfied with the smoothed surface obtained. and click Run.
q
Click a first point. Click again to repeat the smoothing operation if needed. or mesh line. and the Control Points dialog box appears. Open the Smooth1. Simply use the multi-selection capabilities: q Press and hold down the Shift-key and click a first point.CATPart document. click OK in the Control Points dialog box. Only the explicitly selected points are highlighted.FreeStyle Shaper.
Control points are displayed on the surface.
.

FreeStyle Shaper. auto detection. and attenuation. Profiler & Optimizer
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Capabilities are available: q from the contextual menu when right-clicking a control point
q
from the Dashboard are: datum creation.
.

the pointer is over the surface when selecting the edge)
3. the pointer points towards the surface) or from within the surface (i. Move the pointer onto the second surface. appears. only the Diffusion option is available.e.e.
2. Click the surface when the adequate boundary is highlighted.
In case the selected edge relies on more than one support. specifying the continuity between the two elements. or a surface to a curve. Move the pointer over one of the surfaces and click one of its edges. 1.FreeStyle Shaper.
The
tag informs you that there is only one surface to be selected. Some options are only available in FreeStyle Optimizer. that is extend one surface to come up to the other element.
The match is automatically applied. Open the MatchSurface1. 4. You can select edges either from outside the surface (i. Profiler & Optimizer
Matching Surfaces
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In this task you will learn how to match two surfaces.CATPart document. The first surface is recomputed so as to be connected to the second surface. Possible boundaries for the match are highlighted as you move the pointer along. the Please refer to Selecting a Support for further information.
. Click the Match Surface icon .
The Match Surface dialog box is displayed:
In P1 mode.

Furthermore. the deviation is null. trying first to create the match surface in Analytic mode. if both selected curves present the same number of control points. the match is based on the discretization of the selected elements. 6. if not possible. From the Dashboard.FreeStyle Shaper.
q
q
. Profiler & Optimizer
5.
q
Auto: the system optimizes the computation mode.
Information on the match surface is displayed in the Match Surface dialog box: q the number of patches making up the surface
q
the order of the surface to be matched the matching type used (especially useful when working in Auto mode) the delta from the initial surface. in Approximated mode. that is computation mode. and is approximated accordingly. When in P1 mode. Define the matching type. click the Contact Points icon . using the list:
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q
Analytic: available only when the selected curve is an isoparametric curve. The match is computed based on a mathematical formula leading to an exact location of each of the selected curve's control point. only the Auto mode is available. then.
q
Approximated: regardless of the type of the selected surface edges.

Available continuity types are: point.FreeStyle Shaper.
q
q
q
If a continuity type leads to some inconsistencies. a message is displayed on the surface.
.
The tension values are displayed on the element along with a green segment representing the direction and limits of the match surface tangent at its middle-points. click the Tensions icon (P2 only). You can modify the tension values by sliding them along the direction. Profiler & Optimizer
Manipulators are displayed on the connection. normal) at each point of their connection. there is no gap between the surfaces. as the system automatically re-distributes the control point location on the matched surface.e. You can also use the Snap on Geometry option. click on the Continuity icon and right-click
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onto the identifier to edit the continuity constraint on the boundary of the match surface on the target element. Still from the Dashboard. normal) at each point of their connection Curvature: the surfaces share a common curvature and tangent plane at each point of their connection Proportional: similarly to the Tangent option. i. We keep a point continuity on the initial surface. proportional and free.e. Still from the Dashboard. In the example. Capabilities are available from the contextual menu when right-clicking a contact point. free: no constraint is imposed on the curve's control points. 7. using the contextual menu. using the Tension Tuner dialog box. allowing you to interactively define the match limits by simply sliding them along the target curve.
You can right-click the tension value to enter a new value within the 0 to 1 range. tangent. but the longitudinal variation from one point to the other is smoother. q Point: the surfaces share each point of their common boundary. You can edit the contact points by right-clicking to display the contextual menu and choosing the Edit item. Default tensions and tangents are indicated by the Init string. This mode is automatically set for both limits of the matched surface. we impose a tangency constraint on the target surface. surfaces share a common tangent plane (i. curvature. so that you can modify the continuity type:
8.e.
q
Tangent: the surfaces share a common tangent plane (i.

Click on More to display further options: 10. Profiler & Optimizer
Local tangents (identified by the green arrows) are displayed as well enabling you to modify their angle and local tension. You can also choose the Edit angle contextual menu to display the Angle Tuner dialog box. the distance (mm): the maximum distance between the two elements b.
q
q
2. allowing you to dynamically modify them. Check the Control Points option to display the control points and mesh lines on the surface.
9.
See Editing Surfaces Using Control Points to find more about available options. Check the Quick connect checker and orders option: depending on the type of continuity connection. allowing you to specify a given angle.
. three values can be displayed:
a.FreeStyle Shaper. the curvature (%): that is the ratio between both surface curvatures
11. in this case you can modify the value by rightclicking it the first surface tangent (Initial) the target element tangent (Target). the angle (degrees) between the tangents to the surfaces c. Right-click the local tangent to choose from:
q
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a specific value you key in (User). the surface order for each surface d. 1. Click Run to recompute the match surface.

V orders. patch numbers. 12. The Project end points option allows linear projection of the smaller edge. Click OK in the Match Options dialog box. 2. or to modify the constraint in order to edit freely the control points.
The match operation does not modify the input surface. propagates evenly any modification performed using the control points. You then have the choice not to perform the modification.if an exact conversion is possible. V Orders icon .
Numbers indicate the order number of the element along the U and V directions. onto the smaller surface as shown to the left. To the right is the resulting match without the Project end points option:
q
. a new Nurbs surface will replace the input one in order to perform the match. a dialog box is issued warning you that an automatic conversion will be automatically performed before the matching operation: .
The Keep original option enables you to work on a copy of the input surface. This new surface will be added in the specification tree. a message is displayed on the geometry. .if there is a deviation or no exact conversion exists. the Converter Wizard panel appears allowing you to define the approximation according to a tolerance using parameters such as U. and deviation tolerance. the Diffusion option.
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When checked. Right-click a tag number and choose Automatic from the contextual menu to modify the order and the segmentation of the matching surface and reach the desired continuity constraint.FreeStyle Shaper. if selected first. except if you modify its order:
1. as the choice of continuity for example. click the U. Profiler & Optimizer
When a modification is not consistent with constraints previously set.
If you select a frozen surface (a surface with an history) or a non-Nurbs surface as input. From the Dashboard.

contact points. continuity. Profiler & Optimizer
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q
The Project boundary option allows to directly project the first selected boundary onto the second surface. tensions.)
q
The Move on main axis option constrains the matched surface so that its control points can only be moved along the compass' main axis.FreeStyle Shaper.
Checked Move on main axis option
Available capabilities from the Dashboard. attenuation. and furtive display. and/or specified through the FreeStyle Settings. are: datum creation.
. by selection of the surface only. keep original.
Unchecked Move on main axis option The Move on main axis option is only available with FreeStyle Optimizer. auto detection. (You do not need to select a boundary on the target surface.

Some options are only available in FreeStyle Optimizer.
The Multi-side Match dialog box is displayed. Optimize continuities: if checked. the deformation is done optimizing the userdefined continuities rather than according to the control points and mesh lines. Click the Multi-Side Match Surface icon .
q
. other surfaces. The source surface's edges will be deformed to match the target curves on surfaces. taking continuities into account. 1. the deformation is spread over the whole matched surface. Open the MatchSurface2.FreeStyle Shaper. not only to a limited number of control points. Profiler & Optimizer
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Multi-Side Matching
In this task you will learn how to match a mono-cell non relimited surface to at least two. and at most four. Set the deformation options:
q
Diffuse deformation: if checked.
2.CATPart document.

to visualize texts on the geometry. a contextual message helps you select the adequate target curve. It is automatically detected as you move the pointer then highlighted once selected.
6. Continue selecting pairs of source and target curves to be matched.
8.
4.FreeStyle Shaper. Click OK to create the multi-side match surface. Select the target curve for the first selected edge. An arrow is displayed indicating which source edge is to be matched to which target curve.
Then right-click the texts to modify the continuity type (point. tangency. Click Apply to visualize the matched surface. as needed. Select the first edge of the surface to be matched. Profiler & Optimizer
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3.
Note that in case an incorrect edge is detected. Click the Continuity icon
from the dashboard.
. the match is automatically computed. curvature) or to increase/decrease the edge order. If you already selected four source edges and four curves.
5. 7.

e. i. continuity. the two target surface overlap. The match takes into account continuities and order.
. Only a complete surface. that has not been previously relimited. therefore laying on a surface. but also existing geometric configurations. the system automatically relimits the matched surface where the target surfaces overlap:
q
Available capabilities from the Dashboard are: datum creation. For example. Profiler & Optimizer
q
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All source edges must belong to the same surface. Target curves necessary are surface boundaries or isoparametric curves. They cannot be curves created in space. In this case. can be matched. Right-click these texts to choose a new order value. and furtive display (control points are displayed on both the surface to be matched and the target surfaces). Checking the U.
q
A surface can also be matched onto a relimited surface. V Orders icon from the Dashboard. displays texts indicating the resulting
q
q
q
surface order along U and V. auto detection (Snap On Edge option only). in the example below.FreeStyle Shaper.

. Open the Extend1.
The Extend dialog box is displayed. The extended length value is also displayed when moving the manipulator. Profiler & Optimizer
Extending Surfaces
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In this task you will learn how to extend a surface. This means that segments are added to the initial surface. Click the Extend icon . 2. With the Keep segmentation option unchecked: the surface is extended taking the curvature continuity into account. you can preview the modification by a mesh. The surface is then updated when you release the mouse. 1.FreeStyle Shaper. Two working modes are available:
1. and display the surface order as well as the number of segments along both U and V directions. The extended surface is created. that is make it bigger or smaller depending on which side of the manipulator you pull. The extended length value remains.
Checking the Preview button. With the Keep segmentation option checked: the surface is extended according to its initial parameterization. In this mode. Select a surface boundary. A manipulator is displayed.
3. you can hold the Ctrl key down and move the manipulator to generate a symmetric extension. Click OK.CATPart document.
2.

Capability are available from the Dashboard: datum creation and keep original. Profiler & Optimizer
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q
You can also define a step value to extend the surface:
1. Depending on the manipulator's arrow that is clicked and the keyed in value (negative values are allowed) the surface is extended in one direction or the other. Note however that when the Keep Segmentation mode is unchecked.
The Tuner dialog box is displayed. in which you can key the extension step value. the surface can only be extended and not shortened. right-click one of them and choose the Edit contextual menu.FreeStyle Shaper.
.
The Keep this point capability is also available from the contextual menu.
2. The surface is extended by the set step value and the length value is displayed. click the manipulator. Move the pointer back over the manipulator. and pressing and holding the Shift key. When the manipulators are displayed.

3. the Cut (0) text is highlighted.FreeStyle Shaper. 1. Select the surface(s) to be cut. Profiler & Optimizer
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Redefining Surfaces Limits
This task shows how to redefine the limits of one or more surfaces by splitting it along one or more curves. Open the Break1.CATPart document.
The FreeStyle Break dialog box is displayed as well as the Break Report panel and the Tools Palette. Choose the Break type by clicking on the icons on the left. Click the Break icon . Three types are available:
q
Curves by points Curves by curves Surfaces by curves (as in our scenario)
q
q
In the Selection page.
2.
.

If you click on the text.
This panel can also be opened via the Display tab. an error message is issued and the Break Report panel informs you that no element is selected. the corresponding curve is highlighted in red in the 3D geometry.
r
In case of an extrapolation problem. Click the Cutting (0) text and select the cutting curve(s).
r
If there is no selection of cutting elements.
. By default. Profiler & Optimizer
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4.
5.
r
If a red cross is displayed. it means that the problem cannot be managed by the system.FreeStyle Shaper.
The Break Report panel displays all the information regarding the cutting elements. Click Apply. etc). all elements are kept. the corresponding curve is highlighted in green in the 3D geometry. It lists:
q
the cutting elements that can be used for the Break (marked by a green tip). the side of the curve to be extrapolated is circled in red.
q
the cutting elements that cannot be used for the Break (marked by the condition to be applied so that they can be used: projection. extrapolation. If you click on the text.

q
Keep all: all parts of the surface are kept Keep all but this: all parts of the surface are kept except the selected one
q
q
Remove all but this: all parts of the surface are removed except the selected one
7. they are projected (pseudo-intersections) onto it according to the direction set in the Break dialog box:
.
A contextual menu is available on the each part of the surface. Profiler & Optimizer
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6. Click the parts of the surface that you do not want to keep.
Projection
q
no projection: click the Projection text to make the projection optional. the points that do not lie on the trimmed curves will not be projected onto the surface. As a consequence.FreeStyle Shaper.
If certain curves do not lie on the surface. Click the <<Settings text to access advanced settings.

q
The maximum degree variation allowed for each patch of the new surface as compared to patches of the initial surface can be modified. Profiler & Optimizer
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q
Compass: click the compass icon so that the projection is normal to the compass
q
Normal: click the normal icon so that the projection is normal to the element
Relimitation
q
Shorten mesh: curves are not relimited and their limits are redefined.
q
.FreeStyle Shaper. New curves are created. Only 4 edge-patches are created. Click the U Order and the V Order text to edit and modify the values (besides is an example with U and V values set to 8) The U and V order maximum values are set with the Max Order option of the FreeStyle settings.

Click OK to create the break surface. and temporary analysis.
q
.
8.FreeStyle Shaper. Profiler & Optimizer
q
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Keep mesh: curves are relimited and the control points of each initial surface is kept. As a consequence.
Extrapolation
Click the Extrapolation icon if you want the automatic tangency extrapolation of the cutting curves to be optional. insert in a new geometrical set. Available capabilities from the Dashboard are: datum creation. one edge is added.
q
Click the Display>> text to manage the display of the 3D icons and the Break Report panel. The control points of each initial surface is kept. keep original.

Click OK in the dialog box.
3. Click the Untrim icon in the Operations toolbar. icon (see Splitting Geometry for the Generative Shape
The Untrim dialog box is displayed. 1.
2. Profiler & Optimizer
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Restoring a Surface
In this task you will learn how to restore the limits of a surface or a curve when it has been split using the Break Surface or Curve Design workbench).
The dialog box is updated accordingly.FreeStyle Shaper. Open the Untrim1.
.CATPart document. Select the surface which limits should be restored.

It automatically disappears once the operation is complete (progression at 100%).
The initial surface is automatically restored.xxx. Three modes of selection are available:
q
selection of the face: the initial surface is restored
. while the surface is restored. You can perform a local untrim on faces.FreeStyle Shaper.xxx or Curve Untrim. Profiler & Optimizer
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A progression bar is displayed.
The restored surface or curve is identified as Surface Untrim.

If the surface to be restored is closed (in the case of a cylinder) or infinite (in the case of an extrude). Multi-selection is available and allows to create several untrim features in one step. To partially untrim the surface. Therefore. you need to use the Undo command right after the trim. it is the initial surface which is restored.FreeStyle Shaper. All untrim features will appear in the specification tree.
q
q
q
q
. the initial surface and the untrim surface may be identical. You can individually select a vertex or a boundary from the restored surface or curve. Profiler & Optimizer
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q
selection of an inner loop: only this loop is restored
q
selection of the outer loop: only this loop is restored
q
If the surface has been trimmed several times. The datum creation capability is available from the Dashboard. the limits of the untrim feature will be the bounding boxes of the initial surface.

Open the Concatenate2. The Maximum deviation value displayed in the dialog box (see step 5) is computed as the standard distance analysis and therefore is not necessarily the minimum tolerance value to be set in order to concatenate the curves. Click the Concatenate icon . The Concatenate dialog box is displayed.FreeStyle Shaper. This value defines the maximum parametric deviation allowed between the selected elements and the resulting curve when concatenating. provided the tolerance is compatible. The resulting surface is a curvature continuous surface (C2). Set the tolerance value. If not.CATPart document.
3. Profiler & Optimizer
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Concatenating Surfaces
This task explains how to concatenate a two-cell mono-domain FreeStyle surface or two separate contiguous surfaces into a mono-cell surface. a message is issued prompting you to increase the tolerance value. Select the surfaces you wish to concatenate and click Apply. This document contains a set of connex surfaces. A single surface is previewed. 1.
The minimum tolerance value necessary to obtain a result displays as well. 2. with its segment limits in both U and V.
.

. the maximum deviation is also displayed in the dialog box.
6.FreeStyle Shaper. Click More>> in the dialog box.
5. The corresponding information is displayed on the resulting surface. Profiler & Optimizer
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4. Change the tolerance value so that it is compatible to create a single surface. that is:
q
Nu/Nv: number of control points in U and V
q
o: the curve order s: the number of segments in the curve
q
q
the maximum deviation
In case you did not check the Information button. Check the Information option.

FreeStyle Shaper. If the selected elements present a curvature discontinuity you will need to increase the tolerance value accordingly. 8. A surface is created. and so forth.
q
Only two cells. the maximum deviation will increase considerably.
q
If the selected surfaces are not connex (if there is an important gap between the two surfaces) the Apply button is grayed. Check the Auto Update Tolerance button to automatically update the tolerance value in case the value you set is too low. whether in the same element (join for example) or in separate elements (two different cells) can be concatenated at a time. keep original. you need to concatenate the first two cells. Profiler & Optimizer
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7.
q
Available capabilities from the Dashboard are: datum creation. In this case too. then the resulting concatenated surface with another cell. and you cannot create the concatenated surface. This surface is C2 continuous. A minimum result to enable the concatenation is displayed and the concatenation is performed. the result of the concatenation of the initially selected elements (we changed its color to blue for easier identification). To concatenate more. and furtive display.
No message is issued prompting you to increase the tolerance value as the minimum value is set automatically. Click OK in the Concatenate dialog box.
.

Open the FragmentSurface1. Select the surface. Profiler & Optimizer
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Fragmenting Surfaces
In this task you will learn how to fragment multi-segment bodies into mono-segment bodies. allowing the previsualization of the resulting surfaces. along V or in both U and V directions.
4. Choose the breaking options: You can decide to break the surface along U. 3.
. Click the Fragmentation icon in the Shape
Modification toolbar.CATPart document. 1. 2.
The Fragmentation dialog box is displayed.FreeStyle Shaper. The selected surface shows the limits of each segment in solid lines. Click the Keep original icon
from the Dashboard if you want to keep the initial
surface when fragmenting the body.

The surface is fragmented in as many surfaces as there were segments in the initial surface. Click OK. This means that independent surfaces are created. Profiler & Optimizer
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5.
. keep original.
q
Multi-selection is available. we assigned a different color to each of the resulting mono-segment surfaces.FreeStyle Shaper.
q
Available capabilities from the Dashboard are: datum creation. In the example. This function enables you to fragment curves as well (see Fragmenting Curves).

each made of several cells. Profiler & Optimizer
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Disassembling Elements
In this task you will learn how to disassemble multi-cell bodies into mono-cell.
in the
The Disassemble dialog box is displayed.FreeStyle Shaper. or any document containing a multi-cell body. You can select only an edge of a surface. or mono-domain bodies. Open the Disassembling1. Select the element to be disassembled. the system recognizes the whole element to be disassembled. 1.
. whether curves or surfaces.
2. Click the Disassemble icon Shape Modification toolbar.
Here we selected the join made of three elements.CATPartdocument.

and the number of elements to be created according to the disassembling mode are displayed within the Disassemble dialog box. a separate curve is created for each cell. Domains Only: elements are partially disassembled. i. In case of a multi-selection. 4.
q
The number selected elements. for all the selected element. Profiler & Optimizer
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3. Click OK in the dialog box. Choose the disassembling mode:
q
All Cells: all cells are disassembled. In the illustrations. we have colored the resulting curves for better identification. A resulting element can be made of several cells. i.
Results when disassembling all cells Results when disassembling domains only (seven curves are created) (three curves are created) If you wish to create the disassembled elements in a new geometrical set instead of the current geometrical set. while the surface is being disassembled. a progression bar is displayed. each element is kept as a whole if its cells are connex. It automatically disappears once the operation is complete (progression at 100%).e.FreeStyle Shaper. but is not decomposed in separate cells. click the Insert In a New Geometrical Set Dashboard.e. icon from the FreeStyle
.

Profiler & Optimizer
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The selected element is disassembled.FreeStyle Shaper.
. Capabilities available from the FreeStyle Dashboard are datum creation and insert in a new geometrical set. that can be manipulated independently. that is to say independent elements are created. Multi-selection is available.

and the Converter Wizard is not displayed. This approximation is automatically performed when you try to edit a surface using control points. the converter Wizard is displayed allowing you to define the approximation tolerance. 1. Click the Converter Wizard icon . including these created using FreeStyle products.
The Converter Wizard dialog box is displayed allowing you to define the approximation according to a tolerance. Select the surface to be approximated or segmented. 2. and to modify the number of patches (segments) onto any surface. On the geometry. created using other products but FreeStyle.FreeStyle Shaper. a red text is displayed if the tolerance is not respected.
.
q
when the exact conversion cannot be performed. You need to set the values for the different options:
q
Tolerance: that is the deviation tolerance from the initial surface.
Open the Approximate1. that changes to green when the new element is within the specified tolerance. into a NUPBS (Non Uniform Polynomial B-Spline) surface. Profiler & Optimizer
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Approximating/Segmenting Procedural Surfaces
In this task you will learn how to convert any surface. it is done automatically.CATPart document. In this case: q when an exact conversion can be performed.

the system automatically optimizes this option's parameters to comply with the other options' values. the Max order is set to 16 and cannot be modified. in a given direction. or Segmentation. and at least one conversion
q
Provided the Continuity icon
option is active (Tolerance.
Depending on the type of the initial element. Use the contextual menu to select another continuity (point.
q
When one of these options is inactive. The maximum value allowed per patch is defined by the Max order field in the FreeStyle Settings and must be less than or equal to 16. Segmentation: that is the maximum allowed segments along the U and V directions. or curvature
q
q
.
On the selected surfaces. If Single is checked. Orders. One type of continuity can be imposed for each cell of an element. a mono-segment surface is created. Profiler & Optimizer
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Order: that is the maximum allowed order along the U and V directions for each surface patch. when the segmentation options are grayed. This value must be greater than or equal to 2. it must be greater than or equal to 4. segments are delimited by the solid lines. in case of multi-cell elements. In P1 mode.FreeStyle Shaper. every cell has the same continuity constraint.
q
Continuities constraints are applied on the bounding box UV of each cell. Otherwise. a text is displayed indicating what approximation needs to be performed: q CV: the initial surface is not a NUPBS and needs to be approximated using the Converter Wizard parameters
q
EXACT: the initial surface can be converted in exact mode (no parameter needs to be set) Seg: the initial surface already is a NUPBS is active from the Dashboard. a continuity constraint can be imposed identically on the selected surfaces. boundaries are isoparametrics to the selected surfaces. Therefore. tangent.

the continuity tags are displayed in green. Profiler & Optimizer
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continuity) or click the text in the geometry to display the others sequentially. Note that this warning is displayed for information purpose and does not check whether the continuity will be respected or not. a warning is issued and the continuity tags are displayed with the update needed color (here in red) defined in Tools -> Options -> Visualization.FreeStyle Shaper.
If the continuity constraint may be not respected. Click More>> to display more options:
.
3.
If the continuity is certain to be respected (if the order value is sufficient and there is no segmentation constraint).

You can mix the approximation of curves and surfaces. The 3D conversion and 2D icons are grayed as they are useful only for curve conversion. keep original (depending on the selected element).
q
Check the Auto apply button to dynamically update the resulting surface. The Priority check button indicates which of the Orders or Segmentation parameter is taking precedence over the other one. the initial element is duplicated. Profiler & Optimizer
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q
Check the Information option to display further information on the element: r Max: the maximum deviation in relation to the initial element
r
Nu/Nv: number of control points in U and V o: the surface order s: the number of segments in the surface
r
r
q
Check the Control Points option to display the surface's control points. Note that in this case.
q
Multi-selection of surfaces is available. continuities. Use the Exact conversion mode (no parameter needs to be set) on a NUPBS element to display the number of control points.
q
q
q
q
Available capabilities from the Dashboard are: datum creation.FreeStyle Shaper. and number of segments in the curve. The surface modification is taken into account. Click OK. curve order.
. and furtive display. 4.

CATPart document. Open the CopyParameters1. Click the Copy Geometric Parameters icon .
2. Make sure the furtive display is active from the FreeStyle Dashboard. Select the curve that will be used as the template curve. 1.
.
The Copy Geometric Parameters dialog box displays. Control points and segmentation parameters display on the curve.FreeStyle Shaper. Profiler & Optimizer
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Copying Geometric Parameters
This task shows you how to copy the geometric parameters of a curve on one or several curves.

and click Apply to copy the parameters. you can change the template curve still keeping the selected target curves: simply click the Template Curve area in the Copy Geometric Parameters dialog box.FreeStyle Shaper. Click OK. it shows:
q
Input elements: number of selected elements Valid curves: number of curves taken into account
q
5. select the curve. Click Apply to copy the parameters of the template curve on the target curves.
Control points and segmentation parameters also display: you can see that they are different from those of the target curve. it shows:
q
Degree by arc: number of control points Arcs number: number of segments
q
For the target curves. Profiler & Optimizer
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3.
. While in the command.
4.
The Copy Geometric Parameters dialog box updates: For the template curve. Select one or more target curves.

FreeStyle Shaper.
. Profiler & Optimizer
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Only datum and 3D datum curves can be used. Capabilities available from the FreeStyle Dashboard are insert in a new geometrical set and furtive display.

4. Perform this operation onto several surfaces. The boundary is highlighted. Profiler & Optimizer
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Creating a Continuity Constraint
This task shows you how to create a FreeStyle continuity constraint. Make sure the Constraints option is checked in Tools -> Options -> Infrastructure -> Part Infrastructure -> Display tab. 5.
2. Click the surface when the adequate boundary is highlighted.
. so that you are able to see the constraints in the specification tree. Open the Constraint1. that is to connect two or more surfaces or curves and apply a constraint.CATPart document.
3. Click the Continuity Constraint icon .FreeStyle Shaper. Select the edge of the surface to be matched.
The Continuity constraint dialog box displays. Move the pointer onto the second surface. 1.

See Editing Surfaces Using Control Points to find more about available options. allowing you to dynamically modify them. 9.
The continuity constraint feature appears in the specification tree.. Click the text in the geometry to modify the constraint sequentially or use the contextual menu and select the constraint. you need to select them before selecting the surfaces or curves. Click the green arrow to reverse the direction of the constraint and modify the continuity.FreeStyle Shaper. onto the smaller surface. if selected first. Right-click the continuity type to display the contextual menu: you are able to modify the chosen type. May you want to use them. The source surface deforms so that the neighbouring constraints are automatically updated. Check the Control Points option to display the control points and mesh lines on the surface. 7.
Two options are available from the dialog box. q Diffusion: the Diffusion option propagates evenly any modification performed using the control points
q
Project end points: The Project end points option allows linear projection of the smaller edge. 8. under the Constraints node. Profiler & Optimizer
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6.
.

click the Constraints defined in a dialog box icon and set a Distance constraint.
q
q
2. Back in FreeStyle. In Part Design. 3. Constraints created using this command are very similar to the constraints created in the Part Design and the Sketcher workbenches: they are compatible and are solved using a variational approach.
. click the In Model or on Perch icon to switch the compass from the perch to the selected surface.
All the constraints are updated accordingly. using the Quick Compass Orientation toolbar. select a vertex and a point. You can deactivate the constraints using the Deactivate contextual menu.FreeStyle Shaper. Profiler & Optimizer
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q
You can create as many constraints as there are elements. 1. Use the compass to move the surface.

Constraints can only be set on datum elements. under the Constraints node. Profiler & Optimizer
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If you wish to delete a constraint. Refer to the Constraints chapter in the Part Design documentation and to the Setting Constraints chapter in the Sketcher documentation to have further information.
. you need to delete it in the specification tree.FreeStyle Shaper.

e. Analyze using highlights: click the ACA Highlight icon and define stripes or grid lines density. but not retained when exiting the command. spacing. Perform a surfacic curvature analysis: select a surface and specify the display parameters. thickness and sharpness. Check connections between surfaces: select two surfaces. Analyze using highlight lines: select a surface. they are retained in the specification tree for later edition and on the geometry till you reset or delete them. numbers. type.
. color. specify the type of analysis (distance. define the mode and manipulation parameters. tangency. tangency. specify the analysis mode. curvature) and set the analysis parameters. curvature) and set the analysis parameters. Check connections between curves: select two curves. i. and position. Most analyses are permanent in P2 mode only. Use dynamic cutting planes: select a surface. Within the FreeStyle Shaper.). they are present at a time. Profiler & Optimizer
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Analyzing Curves and Surfaces
This chapter deals with curve and surface analysis. Perform a curvature analysis: select a curve or surface boundary. and display parameters. specify the curvature comb parameters (spikes number and length. Analyze using isophotes (P1 mode / P2 mode): specify the isophotes number. etc. thickness. orientation. Analyze the distance between two sets of elements: select a surface and a target element. whereas in P1 mode. Perform a draft analysis: select a surface and specify the display parameters. and specify the highlight type. specify the type of analysis (distance. Manipulate light sources: click the icon.FreeStyle Shaper. etc. specify the cutting planes orientation. Map an environment on a surface: choose the mapping to be reflected onto every element. analyses are elements that need to be explicitly deleted if you do not wish to keep them. The FreeStyle Dashboard tools do not affect the analyses.

or fill operation for example. match. Three types of analyses are available.
1. 2.
r
Distance: the values are expressed in millimeters Tangency: the values are expressed in degrees Curvature: the values are expressed in percentage. Profiler & Optimizer
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Checking Connections Between Surfaces
This task shows how to analyze how two surfaces are connected. Click the Connect Checker icon the Shape Analysis toolbar. The Auto Min Max button enables to automatically update the minimum and maximum values (and consequently all values between) each time they are modified. Select both surfaces to be analyzed. The Connect Checker dialog box is displayed as well as another dialog box showing the color scale and identifying the maximum and minimum values for the analysis type.CATPart document.
. following a blend. in
Check the Internal edges option if you want to analyze the internal connections. the check box is unchecked.FreeStyle Shaper. By default.
r
r
Open the ConnectChecker1.

interference connections may be detected.
q
You can right-click on a color in the color scale to display the contextual menu:
. Topological connections are checked first. you must decrease the Maximum gap value or join the surfaces to be analyzed (see next point)
q
Surfaces are joined (using the Join command for instance) and the Internal edges option is checked.
In the color scale. Be careful not to set a Maximum gap greater than the size of the smallest surface present in the document. Then. 3. In this case. that is all pairs of neighboring surface edges within the tolerance given by the Maximum gap. therefore do not need to be analyzed. All elements apart from a greater value than specified in this field are considered as not being connected. 4. for instance when surfaces have a size smaller the Maximum gap. Tangency or Curvature. Depending on the Maximum gap value. Profiler & Optimizer
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Two cases are available: q Surfaces are isolated. the corresponding pairs of surface edges are checked to detect any geometrical connections within the tolerance given by the Maximum gap. Choose the analysis type to be performed: Distance. Set the Maximum gap above which no analysis will be performed. the Auto Min Max button enables to automatically update the minimum and maximum values (and consequently all values between) each time they are modified. Only geometrical connections are checked. that is all edges shared by two topological surfaces.FreeStyle Shaper.

q
You can also right-click on the value to display the contextual menu:
. because it limits the number of displayed colors in the color scale. However.
. the distribution is done progressively and evenly. you first need to unfreeze the medium value.Use Max/Use Min : it allows you to evenly distribute the color/value interpolation between the current limit values. or use the slider to position the distance value within the allowed range.Edit: it allows you to modify the edition values. and the section of the analysis on which that color was applied takes on the neighboring color.Unfreeze: it allows you to perform a linear interpolation between non defined colors. In this case. . . these limit values are set at a given time. Therefore. meaning that between two set (or frozen) colors/values.FreeStyle Shaper. The unfreezed values are no longer highlighted in green. The Value Edition dialog box is displayed: enter a new value (negative values are allowed) to redefine the color scale. The value is then frozen. and when the geometry is modified after setting them. and displayed in a green rectangle. The Use Max contextual item is only possible if the maximum value is higher or equal to the medium value.
. these limit values are not dynamically updated.No Color: it can be used to simplify the analysis. If not. new settings are available with each new draft analysis.Edit: it allows you to modify the values in the color range to highlight specific areas of the selected surface. rather than keeping it within default values that may not correspond to the scale of the geometry being analyzed. The Color dialog box is displayed allowing the user to modify the color range. Profiler & Optimizer
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. The color scale settings (colors and values) are saved when exiting the command. on the top/bottom values respectively. meaning the same values will be set next time you edit a given draft analysis capability. the selected color is hidden. Only the linear interpolation is allowed. and click OK.

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5. Check the analysis results on the geometry. you can choose a number of visualization and computation options: q the comb: that is the spikes corresponding to the distance in each point
q
the envelope: that is the curve connecting all spikes together Information: that is the minimum and maximum values displayed in the 3D geometry
q
Finally. that is the numbers of spikes in the comb (check the Comb option to see the difference). In automatic mode the comb size is zoom-independent and always visible on the screen. From the Connect Checker dialog box. The number of spikes corresponds to the number of points used for the computation:
. otherwise you can define a coefficient multiplying the comb exact value.
You can also choose the discretization. Each color section indicates on the geometry the distance between the surfaces. the scaling option lets you define the visualization of the comb.
6.FreeStyle Shaper. Here we are analyzing the distance between the surfaces. Check the Information button: Two texts are displayed on the geometry localizing the minimum and maximum values of the analysis as given in the Connect Checker dialog box. This may appear for instance in the case of two non tangent planar surfaces.
There may be a tangency discontinuity while a curvature continuity exists.

An edge is considered as sharp if its tangency deviation is higher than 0.
This mode enables to obtain consistent results with the visualization of sharp edges. specify a deviation of 0. Click the Quick. the colorful area displaying the deviation tolerance between the surfaces shows the continuity whose value is the lowest.. The Connect Checker dialog box changes to this dialog box. To visualize sharp edges. button to obtain a simplified analysis taking into account tolerances.
In P1 mode. The comb is no longer displayed..5 degree minimum. As a consequence.FreeStyle Shaper. In this case the other analysis types are deactivated. The Maximum gap and information are retained from the full analysis. only the quick analysis is available. make sure the View -> Render Style -> Shading with Edges and Hidden Edges option is checked. Coarse: 15 spikes are displayed Medium: 30 spikes are displayed Fine: 45 spikes are displayed
q
q
q
The Full result is only available with the Generative Shape Design 2 product. The maximum deviation value is also displayed on the geometry.
q
You can check the Overlapping button to highlight where. on the common boundary. the two surfaces overlap. The number of selected elements and the number of detected connections are displayed below the color range. In the case you select several types of continuity. the Information button is greyed out. You can use the check button to select one or several analyses (up to three).5 degree. Profiler & Optimizer
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Light: 5 spikes are displayed. or uncheck it to hide the values. 7. To only detect tangency deviations on sharp edges.
q
You can check the Information button to display the minimum and maximum values in the 3D geometry.
.

If you do not wish to create the analysis. such as a Join for example.C1|)
/ ((|C1 + C2|) / 2)
The result of this formula is between 0% et 200%. using the control points for example. The curvature difference is calculated with the following formula:
q
q
q
(|C2 . Profiler & Optimizer
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8. This allows the automatic update of the analysis when you modify any of the surfaces.FreeStyle Shaper. simply double-click it from the specification tree.
The analysis (identified as Surface Connection Analysis. by selecting only one of the initial elements:
q
You can create an analysis on an entire geometrical set simply by selecting it in the specification tree. and choose Delete. For example. If you no longer need the Connection Analysis. Click OK to create the analysis.
q
You can edit the color range in both dialog boxes by double-clicking the color range manipulators (Connect Checker) or color areas (Quick Violation Analysis) to display the Color chooser. Use the spinners to define the deviation tolerances. simply click Cancel. The maximum deviation values on the current geometry are displayed to the right of the dialog box. If you wish to edit the Connection Analysis. the red area indicates all points that are distant of more than 0.
.
q
You can analyze internal edges of a surfacic element.1 mm.
9. right-click Connection Analysis in the specification tree.x) is added to the specification tree (P2 only).

FreeStyle Shaper. or match operation for example. only this mode is available (no quick mode available). You can choose the type of analysis to be performed using the combo: distance. Profiler & Optimizer
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Checking Connections Between Curves
This task shows how to analyze how two curves are connected. 1. Four types of analyses are available. 2. The Connect Checker dialog box is displayed.
In P1 mode. following a blend.
r
Distance: the values are expressed in millimeters Tangency: the values are expressed in degrees Curvature: the values are expressed in percentage Overlapping: the system detects overlapping curves
r
r
r
Open the ConnectChecker2. tangency or curvature. Select both curves to be analyzed.CATPart document.
. Click the Curve Connect Checker icon in the Shape Analysis toolbar. At the same time a text is displayed on the geometry. indicating the value of the connection deviation.

The dialog box changes along with the text on the geometry.FreeStyle Shaper.
4. the text in the geometry disappears because the distance between the two curves is smaller than the set Distance value. Press the Quick button. because the first text displayed is the one for which the set tolerance is not complied with.. Check the Tangency button: A text is displayed on a green background (as defined by default for the Tangency criterion) to indicate that the Tangency criterion is not respected. With our example. or modify the geometry to comply with your needs. You can then increase the Tangency value. Profiler & Optimizer
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This step is P2 only for Wireframe and Surface.
.
3.

Modify the tolerance values. 6. if you check the Curvature value.
The analysis (identified as Curve Connection Analysis. the displayed text indicates that the curvature between the two analyzed curves is greater than the set value. or the geometry to comply with the tolerances. Similarly. Profiler & Optimizer
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5.FreeStyle Shaper.
q
Double-click the Curve Connection Analysis from the specification tree to edit it. simply click Cancel.
The maximum deviation values on the current geometry are displayed to the right of the dialog box. 7. If you do not wish to create the analysis.x) is added to the specification tree. This allows the automatic update of the analysis when you modify any of the curves. using the control points for example (see Editing Curves Using Control Points).
. Click OK to create the analysis. the geometry instantly reflects the compliance with the new value. if you modify the Tangency value to set it to 16 degrees. For example.

FreeStyle Shaper. When the Overlapping button is checked. a text is displayed indicating whether the curves overlap. on the common boundary. In Full mode. other analysis types are deactivated. such as a Join for example. i. but not retained when exiting the command. whereas in P1 mode.
q
The Overlapping mode is not available with the Wireframe and Surface product. it is present at a time.
q
The curve connection checking analysis is permanent in P2 mode only.e. by selecting only one of the initial elements: Use the Overlapping mode to highlight where. the two curves overlap. Profiler & Optimizer
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You can analyze internal edges of a element.
. it is retained in the specification tree for later edition and on the geometry till you reset or delete it.

When analyzing surface boundaries:
q
if you select the surface.
q
Use the Project on Plane checkbox to analyze the projected curve in the selected plane referenced by the compass. Click the Porcupine Curvature Analysis icon . or surface boundaries. Define the analysis parameters in the Curvature Analysis dialog box.
2. the analysis is performed only on this boundary.
1. Profiler & Optimizer
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Performing a Curvature Analysis
This task shows how to analyze the curvature of curves. Select the curve.CATPart document. Open the Analysis1. the analysis is performed on all its boundaries
q
if you select a specific boundary.
.FreeStyle Shaper. Automatically the curvature comb is displayed on the selected curve:
3.

This is the default option. the analysis is performed according to the curve orientation.
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q
4.
.
6.FreeStyle Shaper. This option is particularly useful when the geometry is too dense to be read but the resulting curve may not be smooth enough for your analysis needs. Similarly. You can also decide to halve the number of spikes in the comb clicking as many times as wished the /2 button. Use the spinners to adjust the number of strikes and modify the density. You could just as well double the number of spikes using the X2 button.
5. Profiler & Optimizer
If you uncheck the Project On Plane option. click the /2 button to fine-tune the amplitude (size) of the spikes. and re-compute the analysis curve accordingly.

you do not know how the curve is oriented.
Displaying these values does not modify the analysis. You will get something like this:
8.
. Click Reverse. Check the Automatic option optimizes the spikes length so that even when zooming in or out. Click Curvilinear to switch from the Parametric discretization mode to the Curvilinear analysis.FreeStyle Shaper.
10. the spikes are always visible. Profiler & Optimizer
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7.
9. you will get something like this: That is the analysis opposite to what was initially displayed. This is useful when from the current viewpoint. Check the Logarithm option to display the logarithmic values in the 3D geometry.

Inflection points are displayed only if the Project on Plane and Particular checkboxes are checked. If you check the Particular option. the point will be found on one or other of the curves)
r
r
. you have more options:
r
Keep all inflection points Keep local minimum (corresponds to the absolute minimum under the running point)
r
r
Keep local maximum (corresponds to the absolute maximum under running point) Keep global minimum (in case there are two curves. the point will be found on one or other of the curves) Keep global maximum (in case there are two curves. A Point. if Curvature option is selected.
12. if Radius option is selected.xxx appears in the specification tree. Use the Particular checkbox to display at anytime the minimum and the maximum points.
q
You can right-click on any of the spikes and select Keep this Point to keep the current point at this location. The Inverse Value checkbox displays the inverse value in Radius. or in Curvature. Profiler & Optimizer
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11.FreeStyle Shaper.

. click the icon to display the curvature graph:
The curvature profile and amplitude of the analyzed curve is represented in this diagram. Profiler & Optimizer
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This option is only available in P2 mode in FreeStyle Shaper. For example. Finally. 13. when analyzing a surface. you can use different options to view the analyses.FreeStyle Shaper. and Profiler. by default you obtain this diagram. where the curves color match the ones on the geometry. Optimizer.e. When analyzing a surface or several curves. i. when there are several curvature analyses on elements that are not necessarily of the same size for example.

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q
Same vertical length
: all
curves are displayed according to the same vertical length. The last icon
. and a linear scale for the Curve parameter. as you may move and zoom it within the window. is used to reframe the diagram within the window. values displayed in the diagram are updated.FreeStyle Shaper.
:
Depending on the chosen option. regardless of the scale
q
Same origin
: all curves
are displayed according to a common origin point on the Amplitude scale
q
Vertical logarithm scale all curves are displayed according to a logarithm scale for the Amplitude.

You can slide the pointer over the diagram and the 3D analysis.xxx in the specification tree
q
q
Change color: displays the Color selector dialog box that enables you to change the color of the curve.
The analysis (identified as Curvature Analysis. Profiler & Optimizer
14.
. Click OK in the Curvature Analysis dialog box once you are satisfied with the performed analysis.FreeStyle Shaper.x) is added to the specification tree. Slide the pointer over the diagram to display the amplitude at a given point of the curve. Click the x in the top right corner to close the diagram. 16. you may want to temporarily modify the Depth Effects' Far and Near Limits.
In case of clipping. Right-click a curve and choose one of the following options from the contextual menu:
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q
Remove: removes the curve Drop marker: adds Points.
15. See Setting Depth Effects in CATIA Infrastructure User Guide.

The Distance dialog box is displayed. Profiler & Optimizer
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Analyzing Distances Between Two Sets of Elements
This task shows how to analyze the distance between any two geometric elements. or set of elements.
The distance analysis is computed.CATPart document. 2. Click the Distance Analysis icon in the Shape
Analysis toolbar.
. Each color identifies all discretization points located at a distance between two values.FreeStyle Shaper. as defined in the Color Scale dialog box. Click Second set and select a second element. Open the DistanceAnalysis1. Select an element. or between two sets of elements. 1.
3. or set.

provided the Color scale checkbox is checked. Two analysis modes are available. q If you check the Running point option. and discretizes the one with the smallest dimension. The projection is visualized and the value is displayed in the geometry area. as shown here. Use the Invert Analysis button to invert the computation direction. you need to move the pointer over the discretized element to display more precise distance value between the point below the pointer and the other set of elements. in the case of planar curves for example. Therefore the distance is always expressed with a positive value when analyzing the distance between two curves. This is obvious when a low discretization value is set. when inverting the computation direction does not make sense. there is no negative values possible as opposed to when analyzing the distance between a surface and another element. only two directions are defined. Profiler & Optimizer
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q
When computing the distance between two curves.
. when one of the elements is a plane for example. When selecting a set of element. with corresponding color ramps.
q
q
In some cases. the Invert Analysis button is grayed. Indeed. if needed. surfaces present an orientation in all three space directions whereas.1 for curves. the system compares the greatest dimension of all elements in each set. The element which dimension is the smallest (0 for points.FreeStyle Shaper.
Note that the analyzed point is not necessarily a discretized point in this case. 2 for surfaces for example) is automatically discretized.

Whichever mode you choose the use of the color scale is identical: it lets you define colors in relation to distance values. therefore attributing a color to all elements which distance falls into to given values. Profiler & Optimizer
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a. Full (P2 only): activated by the Full color range icon. it
provides a complete analysis based on the chosen color range. Limited: activated by the Limited color range . with only three values and four colors.FreeStyle Shaper. q The Auto Min Max button enables to automatically update the minimum and maximum values (and consequently all values between) each time they are modified. This allows you to see exactly how the evolution of the distance is performed on the selected element. it provides a simplified analysis.
.
b. You can define each of the values and color blocks.

because it limits the number of displayed colors in the color scale. The Color dialog box is displayed allowing the user to modify the color range.Unfreeze: it allows you to perform a linear interpolation between non defined colors.Edit: it allows you to modify the values in the color range to highlight specific areas of the selected surface. .No Color: it can be used to simplify the analysis. The unfreezed values are no longer highlighted in green.
. and the section of the analysis on which that color was applied takes on the neighboring color.FreeStyle Shaper. the selected color is hidden. Profiler & Optimizer
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q
You can right-click on a color in the color scale to display the contextual menu:
. In this case.
q
You can also right-click on the value to display the contextual menu:
.

FreeStyle Shaper. and displayed in a green rectangle. rather than keeping it within default values that may not correspond to the scale of the geometry being analyzed. The value is then frozen. Therefore. Profiler & Optimizer
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. and click OK. The color scale settings (colors and values) are saved when exiting the command. on the top/bottom values respectively. the distribution is done progressively and evenly. If not. these limit values are set at a given time. you first need to unfreeze the medium value. Only the linear interpolation is allowed. meaning that between two set (or frozen) colors/values. these limit values are not dynamically updated. new settings are available with each new distance analysis.Use Max/Use Min : it allows you to evenly distribute the color/value interpolation between the current limit values. and when the geometry is modified after setting them.Edit: it allows you to modify the edition values. Set the distance analysis type (we checked the Auto Scale button and unchecked the Min/Max values button):
Projection Space
The Projection Space area helps you define the preprocessing of the input elements used for the computation. meaning the same values will be set next time you edit a given distance analysis capability. However. This frame is only available when analyzing distances between curves. or use the slider to position the distance value within the allowed range. The Value Edition dialog box is displayed: enter a new value (negative values are allowed) to redefine the color scale.
. . 5. The Use Max contextual item is only possible if the maximum value is higher or equal to the medium value.

Measurement Direction
The Measurement Direction area provides options to define how set the direction used for the distance computation.
. Profiler & Optimizer
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q
3D
: elements are not
modified and the computation is done between the initial elements.
q
Projection according to the X
.Y
.
q
Projection according to the compass current orientation between the projection of selected elements.FreeStyle Shaper.
: the computation is done
q
Planar distance
: the
distance is computed between a curve and the intersection of the plane containing that curve. or Z
axis: the computation is done
between the projection of selected elements.

. The latter
allows to visualize the distance evolution.
6.FreeStyle Shaper.
q
Direction according to the X . Profiler & Optimizer
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q
Normal distance
: the
distance is computed according to the normal to the other set of elements. Click the
icon to display the 2D diagram distance analysis window. or Z axis.
q
Direction according to the compass current orientation .Y .

FreeStyle Shaper.
This option is only available if the Color Scale checkbox is checked.
q
Statistical distribution: to display the percentage of points between two values. Profiler & Optimizer
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q
Color scale: to display the Color Scale dialog box whether the full or the limited color range.
.

You can further choose to: r set a ratio for the spike size
r
choose an automatic optimized spike size (Auto scale) invert the spike visualization on the geometry display the envelope.
q
Points: to see the distance analysis in the shape of points only on the geometry (The Spikes button is unchecked)
q
Spikes: to see the distance analysis in the shape of spikes on the geometry.FreeStyle Shaper. that is the curve connecting all spikes together
r
r
q
Use the Texture option to check the analysis using color distribution.
. Profiler & Optimizer
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Min/Max values: to display the minimum and maximum distance values and locations on the geometry.

. providing this set is discretized. see Improving Performances.FreeStyle Shaper.01). The texture mapping is computed on the discretized surface. the 3D Accuracy -> Fixed option should be set to 0. Statistical distribution. Otherwise a warning is issued. Profiler & Optimizer
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This option is only available with surfacic elements in at least one set. and Points cannot be visualized when using the Texture option. If you extend the curve for instance. and the discretization option should be set to a maximum (in CATIA Infrastructure User Guide. this ratio is kept. Check the Material option in the View -> Render Style -> Customize View command to be able to see the analysis results on the selected element.
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Start and end points are defined by a ratio of curve length between 0 and 1. The visualization mode should be set to Shading with Texture and Edges. Use the Curve Limits option to relimit the discretized curve. The distance is computed from this discretized set to the other set. Two manipulators appear at both extremities of the curve: they let you define new start and end points on the curve. Min/Max values. It is not advised to use it with planar surfaces or ruled surfaces.

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Use the Discretization option to reduce or increase the number of points of the second set of elements taken into account when computing the distance. Profiler & Optimizer
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Use the Max Distance option to relimit the distance: for example. thus improving the performances. in the case of a large cloud of points. in normal projection type.x) is added to the specification tree. the distances are computed as the normal projection of each point of the first cloud onto the triangle made by the three points closest to that projection onto the second cloud. using the Invert Analysis button does not necessarily gives symmetrical results. Be careful when using the Automatic trap option with certain cloud configurations.
You can calculate the minimum distance between two curves along a direction using the Knowledge Expert product. In this case. refer to the Knowledge Expert's User's Guide.FreeStyle Shaper. as the automatic trap may remove too many points to generate consistent results.
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The auto detection capability is available from the FreeStyle Dashboard.
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Even though you exit the analysis. all the elements included in this geometrical set are automatically selected too. set the value to 150mm. Automatic trap: to delimit the second set of points to be taken into account for the computation. For further information. This is like a shortcut allowing you to modify one of the analyzed elements. Click OK to exit the analysis while retaining it. 8. Functions Package. which leads to a dynamic update of the distance analysis. Measures chapter. it is best to deactivate the check button. the color scale is retained till you explicitly close is. while viewing the set values/colors at all times and without having to edit the distance analysis. Reference. The maximum value is displayed accordingly on the geometry. When you select the geometrical set as an input in the specification tree.
. As it is a projection. When analyzing clouds of points. such as spiralling clouds of points for example.
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The analysis (identified as Distance Analysis.

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Using Dynamic Cutting Planes
This task shows how to analyze a surface using parallel cutting planes. A reference plane is displayed along with the default number of cutting planes. Independent planes) The boundaries of the set of planes (available in Parallel Planes mode only): r Automatic: the analysis is performed based on all selected surfaces bounding boxes. Open the CuttingPlane1. 2. Click the Cutting Planes icon in the Shape
Analysis toolbar. You can define analysis parameters from this dialog box.CATPart document. This analysis is dynamic. meaning that you can interactively modified a number or parameters to fine-tune the analysis. From these curves. and the corresponding projected lines onto the selected surface. The cutting planes are evenly distributed within
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. using the three icons (Parallel Planes.
The Cutting Plane dialog box is displayed. The intersection of the planes with the surface is represented by curves on the surface.FreeStyle Shaper. Planes perpendicular to curves. 1. you can visualize the porcupine analysis. that is:
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The plane in which the analysis is to be performed. Select the surfaces to be analyzed.

the number of planes depends on the size of the analyzed area. defines the distance at which the first (start) and last (end) cutting planes are located on the reference plane axis. This option is only available in Parallel Planes and Planes perpendicular to curves mode. In the latter case.FreeStyle Shaper.
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Number/Step: choose whether you have a set number of planes or a distance (step) between two planes.
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this area.
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Options facilitating
. one being necessarily located on the reference plane if the Step option is active.

except that it displays spikes for each intersection curve.
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The compass moves to the reference plane center. Activates/hides the representation of the cutting planes 2. Click the Parallel planes icon .
3. The result is similar to using the Porcupine curvature analysis. Profiler & Optimizer
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the analysis reading:
1.FreeStyle Shaper. See Performing a Curvature Analysis. Activates the display of the curvature comb (Curvature option)
If you click the Settings button. the Curvature Analysis dialog box is displayed. and from then you can manipulate the reference plane.

Planes are added to the specification tree. select a curve and click the Planes perpendicular to curves icon. Select a reference curve 2.FreeStyle Shaper. This option is only available with the Planes perpendicular to curves type.
Using the Planes perpendicular to curves type. Check the On curve option You can create several planes: rightclick the reference plane and select Keep this plane from the contextual menu.
. you can check the On curve option in the Number/Step area to create perpendicular planes. Profiler & Optimizer
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If you want to perform an analysis in planes perpendicular to curves. 1.

The planes are automatically relocated. set the Step value to 30. Profiler & Optimizer
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If you want to perform an analysis in independent planes. See Stacking Commands for further information. Each created plane is added to the current list of planes used for the analysis. click the Independent planes icon.
4.FreeStyle Shaper.
. Activate the Manual mode.
You can use the contextual menu on the Independent planes icon to create the a plane. and the Start value to -150 and End value to 150.

Click Cancel to interrupt the function and remove the analysis. Click OK in the Cutting Plane dialog box. so that it is dynamically updated when deforming the surface.x) is added to the specification tree.
The analysis (identified as Cutting Plane Analysis.
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The Keep this point option is also available from the contextual menu. Right-click the intersection curves to actually create the curve on the analyzed surface.FreeStyle Shaper. Profiler & Optimizer
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5. You can choose to create only the curve over which the pointer is (Keep this intersection curve option) or to "drop" all curves onto the element (Keep all intersection curves option).
.
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Click OK to interrupt the function while keeping the analysis on the surface. when you have finished the analysis.

the angle should be computed between the first direction of the compass and the tangent to the intersection.
. Select the highlight type:
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Tangent: the compass plane intersects the surface at a given point. Click the Highlight Lines Analysis icon .
3. The tangent in each point of the created line is defined through rotations of the angle pitch. Profiler & Optimizer
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Analyzing Using Highlight Lines
This task shows you how to create and visualize curves on surfaces in order to analyze the surface shape and curvature variations.FreeStyle Shaper. Select one or more surfaces to be analyzed. Open the HighlightLines1.
2.
The Highlight Lines dialog box displays.CATPart document. Then the tangent to this intersection is calculated. 1. Therefore.

You can right-click a line to convert it into a curve.x) is added to the specification tree. 4. The normal to the surface in each point of the created line has the same angle pitch in a specified direction. Click OK when you have finished the analysis. Two options are available from the contextual menu:
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Keep this highlight line Keep all highlight lines
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The created curve(s) appears in the specification tree as a datum element.
. representing the value between the selected direction and the normal or tangent to the surface.
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Normal: the angle should be computed between the Z compass direction and the normal to the surface. Key in an angle.FreeStyle Shaper.
The analysis (identified as Highlight Lines Analysis.

No warning message is issued as long as no element is selected.
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You can right-click on a color in the color scale to display the contextual menu:
. Select a surface. Open the SurfacicAnalysis1. set the 3D Accuracy -> Fixed option to 0.
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Uncheck the Highlight faces and edges option in Tools -> Options -> General -> Display -> Navigation to disable the highlight of the geometry selection.1 dialog box showing the color scale and identifying the maximum and minimum values for the analysis is displayed too. It gives information on the display (color scale).
The Surfacic curvature dialog box is displayed. 1.
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You can now perform an analysis on the fly even if the Material option is not checked. Profiler & Optimizer
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This command is not available with the Generative Shape Design 1 product. Used in Part Design workbench. Click the Surfacic Curvature Analysis icon in the Shape Analysis toolbar. Check the Material option in the View -> Render Style -> Customize View command to be able to see the analysis results on the selected element. The Surfacic Curvature.
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The discretization option should be set to a maximum: in Tools -> Options -> Display -> Performances. this command requires the configuration mode.FreeStyle Shaper. 2.
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This task shows how to analyze the mapping curvature of a surface.CATPart document. the draft direction and the direction values. and the analysis is visible on the selected element.01.

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. these limit values are set at a given time.No Color: it can be used to simplify the analysis.
. on the top/bottom values respectively. and displayed in a green rectangle.Interpolation: by default the interpolation is linear. If not. we defined minimum and maximum values and used the on the fly option (except for Limited and Inflection Area type)
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Gaussian
. .Use Max/Use Min: it allows you to evenly distribute the color/value interpolation between the current limit values. The Color dialog box is displayed allowing the user to modify the color range. or use the slider to position the distance value within the allowed range. The unfreezed values are no longer highlighted in green. and click OK. rather than keeping it within default values that may not correspond to the scale of the geometry being analyzed. Select the type analysis:
In the following examples.
Type
3.
. these limit values are not dynamically updated. because it limits the number of displayed colors in the color scale.
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You can also right-click on the value to display the contextual menu:
. and the section of the analysis on which that color was applied takes on the neighboring color.Edit: it allows you to modify the edition values.FreeStyle Shaper.Edit: it allows you to modify the values in the color range to highlight specific areas of the selected surface. and when the geometry is modified after setting them. you first need to unfreeze the medium value. In this case. the selected color is hidden. The Value Edition dialog box is displayed: enter a new value (negative values are allowed) to redefine the color scale. The value is then frozen. Therefore. .Unfreeze: it allows you to perform a linear interpolation between non defined colors. The Use Max contextual item is only possible if the maximum value is higher or equal to the medium value.

Note that these inflection lines are always created within the green area.1 dialog box. as well as the minimum and maximum curvature values and the minimum and maximum curvature directions. Profiler & Optimizer
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Limited: the quick mode is displayed and the Limited Radius type is selected. This option enables to perform a local analysis.FreeStyle Shaper. The value is automatically updated in the color scale. The curvature and radius values are displayed under the pointer.
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Inflection Area: enables to identify the curvature orientation:
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In green: the areas where the minimum and maximum curvatures present the same orientation In blue: the areas where the minimum and maximum curvatures present opposite orientation
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See also Creating Inflection Lines.e. the display is dynamically updated. i. Activate the On the fly checkbox and move the pointer over the surface.
Display options
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Uncheck the Color Scale checkbox to remove the Surfacic Curvature Analysis.
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. you are able to modify the radius value using the up and down arrows. when the curvature orientation is changing. In the Surfacic curvature dialog box. The values are expressed in the units set in using the Tools -> Options -> General -> Parameters -> Units tab. As you move the pointer over the surface.

keep the point corresponding to the minimum value .
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Activate the 3D MinMax checkbox to locate the minimum and maximum values for the selected analysis type.FreeStyle Shaper. You cannot snap on point when performing a local on the fly analysis. It allows you to : . The On the fly analysis can only be performed on the elements of the current part.keep the point corresponding to the maximum value A Point.xxx appears in the specification tree.
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In P1 mode. Profiler & Optimizer
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The displayed values may vary from the information displayed as the Use Max / Use Min values.keep the point at this location (under the pointer) . It is not available with the Inflection Area analysis type. Right-click a point to display the contextual menu. this contextual menu is not available. as it is the precise value at a given point (where the pointer is) and does not depend on the set discretization.
.

This capability is not available in P1 mode. the Minimum and Maximum values are updated in the Surfacic Curvature.x) is added to the specification tree.
The analysis (identified as Surfacic Curvature Analysis.FreeStyle Shaper. click OK in the Surfacic Curvature Analysis dialog box. This allows you to check the impact of any
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If you double-click the Surfacic Curvature Analysis.
4. You can display the control points by clicking the modification on the surface.
. icon.xxx in the specification tree.
These options are not available with the Limited and Inflection Area analysis types. still viewing the surfacic curvature analysis.1 analysis but not in the color scale. Here are examples using the 3D MinMax capability. Once you have finished analyzing the surface. Profiler & Optimizer
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Check the Radius Mode analysis option to get analysis values as radius values.

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To update the values in the color scale. refer to the Customizing Units chapter in the CATIA Infrastructure User's Guide documentation.
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Surfacic curvature analyses can be performed on a set of surfaces. The analysis results depend of the current object. it cannot be selected simultaneously for another analysis.FreeStyle Shaper. May you want to change the scope of analysis. To do so. use the Define in Work object contextual command. right-click the minimum value and the maximum value and select respectively Use Min / Use max from the contextual menu. If an element belongs to an analysis. You can customize the values expressed in the color scale and in the 3D geometry. it may happen that the analysis results are not visible.
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. In some cases. or perform an update on the involved geometric element(s). For further information. then define or redefine the default units. select the Tools -> Options -> General -> Parameters and Measures -> Unit command. even though the rendering style is properly set. Check that the geometry is up-to-date. you need to remove the current analysis by deselecting the element to be able to use it again.

Check the Material option in the View -> Render Style -> Customize View command to be able to see the analysis results on the selected element.
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This task shows how to analyze the draft angle on a surface. Click the Draft Analysis icon Shape Analysis toolbar.01. Select a surface. this command requires the configuration mode. These values are expressed in the unit as specified in Tools -> Options -> General -> Parameters -> Unit tab. Uncheck the Highlight faces and edges option in Tools -> Options -> Display -> Navigation to disable the highlight of the geometry selection. It simplifies the analysis in that it displays only three color ranges. This type of analysis is performed based on color ranges identifying zones on the analyzed element where the deviation from the draft direction at any point. It is highlighted. 2.1 dialog box showing the color scale and identifying the maximum and minimum values for the analysis is displayed too.FreeStyle Shaper. Otherwise a warning is issued.
Mode option
The mode option lets you choose between a quick and a full analysis mode.
. Used in Part Design workbench. You can modify them by clicking on their corresponding arrow or by entering a value directly in the field. It gives information on the display (color scale). These two modes are completely independent.CATPart document. The Draft Analysis command enables you to detect if the part you drafted will be easily removed. 1. set the 3D Accuracy -> Fixed option to 0. The Draft Analysis. Open the DraftAnalysis1. corresponds to specified values. in the
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The Draft Analysis dialog box is displayed.
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The visualization mode should be set to Shading With Edges in the View -> Render Style command The discretization option should be set to a maximum: in Tools -> Options -> Display -> Performances. Profiler & Optimizer
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This command is not available with the Generative Shape Design 1 product. The default mode is the quick mode. the draft direction and the direction values.

Edit: it allows you to modify the values in the color range to highlight specific areas of the selected surface. Profiler & Optimizer
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Quick mode
Full mode
In P1 mode.FreeStyle Shaper. Therefore.
. on the top/bottom values respectively. and click OK.
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You can right-click on a color in the color scale to display the contextual menu:
. only the quick mode is available. The Value Edition dialog box is displayed: enter a new value (negative values are allowed) to redefine the color scale. The unfreezed values are no longer highlighted in green. and displayed in a green rectangle.Unfreeze: it allows you to perform a linear interpolation between non defined colors.Use Max/Use Min : it allows you to evenly distribute the color/value interpolation between the current limit values. and when the geometry is modified after setting them. these limit values are not dynamically updated.
. . or use the slider to position the distance value within the allowed range. these limit values are set at a given time. rather than keeping it within default values that may not correspond to the scale of the geometry being analyzed. The value is then frozen. .No Color: it can be used to simplify the analysis.Edit: it allows you to modify the edition values. because it limits the number of displayed colors in the color scale. and the section of the analysis on which that color was applied takes on the neighboring color. In this case. The Color dialog box is displayed allowing the user to modify the color range. the selected color is hidden.
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You can also right-click on the value to display the contextual menu:
.

do not forget to invert locally the normal direction via the Inverse button. Note that you can activate the On the fly option even when not visualizing the materials. the draft direction is inverted for each element when the button is clicked.
Display option
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Uncheck the Color Scale checkbox to remove the Draft Analysis.
This dialog box only appears in edition mode.
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Activate the On the fly checkbox and move the pointer over the surface. the display is dynamically updated. It is expressed in the units set in using the Tools -> Options -> General -> Parameters -> Units tab.
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The color scale settings (colors and values) are saved when exiting the command. circles are displayed indicating the plane tangent to the surface at this point.
In case of an obviously inconsistent result. and the tangent (blue arrow).1 dialog box. you first need to unfreeze the medium value. the distribution is done progressively and evenly.
. This option enables you to perform a local analysis.
Furthermore. Only the linear interpolation is allowed. However. The manipulator on the draft direction allows you to materialize the cone showing the angle around the direction. If not. identifying the normal to the surface at the pointer location (green arrow).
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Click the Inverse button to automatically reverse the draft direction:
When several elements are selected for analysis. As you move the pointer over the surface. new settings are available with each new draft analysis. Arrows are displayed under the pointer. The displayed value indicates the angle between the draft direction and the tangent to the surface at the current point. meaning that between two set (or frozen) colors/values. meaning the same values will be set next time you edit a given draft analysis capability. the draft direction (red arrow). The On the fly analysis can only be performed on the elements of the current part.FreeStyle Shaper. It gives you the tangent plane and the deviation value. Profiler & Optimizer
The Use Max contextual item is only possible if the maximum value is higher or equal to the medium value.

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Direction in the cone Right-click the cone angle to display the Angle Tuner dialog box. the value is automatically updated in the color scale and in the geometry.
Direction out of the cone
Please note that you cannot modify the angle below the minimum value or beyond the maximum value.FreeStyle Shaper.
Full mode
Quick mode
. When you modify the angle using the up and down arrows.

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In P1 mode. the Keep Point option is not available.
Using the compass manipulators
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Selecting a specific direction
Click the Compass icon
to define the new current draft direction.
You can display the control points by clicking the Control Points
icon. when available. then allowing you to
check the impact of any modification to the surface on the draft analysis.
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Click the Locked direction icon
.
Direction
By default the analysis is locked. a plane or planar face which normal is used).FreeStyle Shaper.xxx appears in the specification tree. yet the draft analysis is still visible. Profiler & Optimizer
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Right-click the Direction vector to display the contextual menu. In P1 mode. It allows you to:
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hide / show the cone hide / show the angle hide / show the tangent lock / unlock the analysis position keep the point at this location A Point.
The compass lets you define the pulling direction that will be used from removing the part. or use the
compass manipulators. meaning it is done according to a specified direction: the compass w axis.
. and select a direction (a line. the default analysis direction is the general document axis-system's z axis.

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3. A draft analysis can be performed just as well on a set of surfaces. and redisplayed when you select the Draft Analysis icon again. May you want to change the scope of analysis. it may happen that the analysis results are not visible. or perform an update on the involved geometric element(s). Check that the geometry is up-to-date. when selecting the direction. even though the rendering style is properly set. it cannot be selected simultaneously for another analysis. This capability is not available in P1 mode. If an element belongs to an analysis.
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Note that settings are saved when exiting the command. you need to remove the current analysis by deselecting the element to be able to use it again.x) is added to the specification tree. Once you have finished analyzing the surface. In some cases. use the Define in Work object contextual command. click OK in the Draft Analysis dialog box. Be careful. The analysis (identified as Draft Analysis. not to deselect the analyzed element. The analysis results depend of the current object.

.jpg. Check the Material option in the View -> Render Style -> Customize View command to be able to see the analysis results on the selected surface. The Environment Mapping dialog box is displayed:
2.FreeStyle Shaper. Open the Analysis1. 5. Define the type of mapping to be applied using the drop-down list.
. Set the reflectivity coefficient which defines the transparency of the texture using the slider.bmp.
You can also import an image file (of type . . Click OK.rgb) using the Browse icon 3. Select one or more surfaces and apply different image definitions.x) is added to the specification tree. 1.
4.
The analysis (identified as Environment Mapping Analysis. It could look like this:
.
You can click the
icon to perform a global analysis.CATPart document. Click the Environment Mapping icon in the Shape Analysis toolbar. Profiler & Optimizer
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Mapping an Environment on a Surface
This task explains how to map a sample environment onto a surface generated using the FreeStyle Shaper. The surfaces automatically reflect your mapping definition. The preview area lets you fine-tune these parameters.

Click the Isophotes Analysis icon in the Shape Analysis toolbar. It is a tool for the analysis of the element state.FreeStyle Shaper.CATPart document. Open the Analysis1. Isophotes are variable black stripes applied to the surface and used for analysis purposes. see Performance: the 3D Accuracy -> Fixed option should be set to 0. Profiler & Optimizer
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Analyzing Using Isophotes (P1 Mode)
This task explains how to apply isophotes on a surface.01.
.
The Isophotes_Mapping dialog box is displayed:
2. 1. The discretization option should be set to a maximum (in CATIA Infrastructure User Guide. Define the analysis parameters using sliders: number of stripes width color transition (smooth or sharp)
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The preview area is directly applied on the 3D screen and lets you finetune these parameters.

The visualization is displayed directly on the surface in the Preview area.FreeStyle Shaper. You do so by clicking one of these spheres until you find the right orientation.
The surface automatically reflects your mapping definition. It could look like this:
. a green sphere
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If you want to orientate perpendicularly the surface. Define the orientation in space using three manipulators: the two yellow spheres enable you to perform any orientation of the surface in space. click the Clean button. just click one of these three spheres. If you want to reset the orientation perpendicularly to the Z axis. Profiler & Optimizer
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3. If you want to undo the mapping on the 3D screen. click the Reset button.

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With a same mapping definition. the isophotes source is fixed.
. Indeed. the mapping will differ if you move the element in space. and the same element will present a different mapping when moved in relation to that source.

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Analyzing Using Isophotes (P2 Mode)
This task explains how to apply isophotes on a surface. 1. 3. Isophotes are variable black stripes applied to the surface and used for analysis purposes.01). use the Define in Work object contextual command. Open the IsophotesMapping1. The discretization option should be set to a maximum (in CATIA Infrastructure User Guide.FreeStyle Shaper. Define the mapping type:
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Cylindrical mode
. in the
2. May you want to change the scope of analysis.
The analysis results depend of the current object. see Performance: the 3D Accuracy -> Fixed option should be set to 0. The Isophote Analysis dialog box is displayed.CATPart document. Select one or more surfaces to be analyzed. Click the Isophotes Analysis icon Shape Analysis toolbar. Otherwise a warning is issued. It is a tool for the analysis of the element state. Check the Materials option in the View -> Render Style -> Customize View command to be able to see the analysis results on the selected element.

Define the options:
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Global
: lets you analyse the whole part.
Uncheck this icon to perform the analysis element by element. Profiler & Optimizer
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Spherical mode
4.
.
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Compass
: flips the compass to the model and
lets you move the compass in the 3D geometry to define the orientation.
It is advised to use the Global mode for a global selection rather than using a trap.FreeStyle Shaper.

5.FreeStyle Shaper. Stripes are recalculated each time you move the mouse. Profiler & Optimizer
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View
: lets you use the screen definition to
define the orientation. Define the analysis parameters using sliders:
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number of stripes
Few stripes
Many stripes
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width
Black thick stripes
Black thin stripes
.

The analysis (identified as Isophotes Mapping Analysis. It could look like this:
. Profiler & Optimizer
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color transition
Sharp color transition
Smooth color transition
The preview area is directly applied on the 3D screen and lets you fine-tune these parameters.x) is added to the specification tree. The surface automatically reflects your mapping definition. 6.FreeStyle Shaper. Click OK when you have finished the analysis.

You do not need to select the part in the specification tree as the analysis works globally on the part.80
Here is an example the following values Grid and Global Density=80 Thickness=0. 2. Density: defines the number of stripes or grid lines. Dependent on the angle. Sharpness: defines the sharpness of stripes or grid lines (soft or hard color transition).
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Here is an example the following values Grid and Global Density=50 Thickness=0. 1. Make sure the Shading and Material visualization options are active by selecting the Customize View icon toolbar. it sets the color at this surface position. the resulting stripe is the silhouette line related to the predefined direction. The plane tool u and v direction. Angle: highlights are distributed per angle.FreeStyle Shaper. it switches to the Stripes mode: the plane tool normal is the predefined direction.30
.30 Sharpness=0. are used as predefined directions in grid mode.
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Global: the whole part is highlighted. If the angle is 90 degrees. It analyses the angle between surface normals and a predefined direction. Profiler & Optimizer
Analyzing Using Highlights
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This task shows how to perform an analysis of the surfaces quality of shaded highlights. All positions with the same angle between surface normal and predefined direction get the same shading color. Open the Highlights1. Click the Highlight icon . in the View mode
The Highlights dialog box displays. Define the display options:
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Grid: two predefined directions define a grid of stripes (not necessarily perpendicular) on the surface.CATPart document. If you uncheck the Grid options. Thickness: defines the thickness of stripes or grid lines.70 Sharpness=0.

As a result in grid mode the silhouette line of the plane tool u direction and the silhouette line of the plane tool v direction are crossing at the plane tool origin
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Define the rotation mode of the 3D tool:
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Dynamic: normal dynamic rotation mode Discrete: the rotation of the tool snaps to certain relative grid angles.70 Sharpness=0. The grid value defines the specific rotation angle
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Define the rotation value by entering a value or using the spinners
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Here is an example the following values Grid.30
3. 3D curve endpoint).FreeStyle Shaper. the direction is adapted to the surface normal or curve tangent
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Curve: the plane tool snaps on a curve or surface edge.
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Define the snap mode to snap tool position and optionally orientation on geometry
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Off: no snap mode Vertex: the plane tool snaps on a vertex. and Angle Density=80 Thickness=0. Dependent on the vertex (surface corner.
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Grid: the rotation of the tool snaps to certain absolute grid angles. Right-click the plane tool to display the Highlights Properties. As a result in stripes mode the silhouette line of the plane tool normal crosses the edge at the plane tool origin
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Surface: the plane tool snaps on a surface and adapts the surface normal.30
Here is an example the following values Global and Angle Density=80 Thickness=0.70 Sharpness=0.
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Static: the rotation is activated by a mouse click on the corresponding rotation handle of the tool. Global.

FreeStyle Shaper.
. y and z components of the current coordinate system
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Coordinates: absolute position of the tool in the model coordinate system
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Define the numerical feedback of the 3D tool:
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Distance 3D: direct distance between the start position of the translation and the current position
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Distance XYZ: distance shown in x. Click OK to create the analysis. please refer to the CATIA Automotive Class A documentation.
For further information.

Now if you position your mouse over an arc. the light source is rotated along its axis. a predefined dotted circle is displayed.
1. Select the light source mode:
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Attached to Viewpoint: the light source is fixed to the screen and the model can rotate independently to the light source position. Use the arrows to define the rotation.FreeStyle Shaper. If you drag your mouse along that circle. the target):
When you point at an arrow.e.
2.
The Light Source Manipulation dialog box opens. Click the Light Source Manipulation icon
.
r
Attached to Model: the light source is fixed in the reference axis of the current model. a predefined dotted circle will also appear.
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Manipulating Light Sources
This task shows you how to manipulate light sources along predefined circles that are centered on the light target.CATPart document. 3.
Open the LightSource1.
Manipulators appear in the 3D geometry and the red arrow represents the light direction (i.

Right-click a manipulator and select one of the following contextual commands:
. By default. Drag the mouse long the circle handler to change the position of the light source origin along the selected arc:
Note that you can move the light position step-by-step by pressing the Ctrl key then dragging your mouse simultaneously. 5.FreeStyle Shaper. the light source is rotated 10 degrees by 10 degrees but you can modify this value if needed via the Direction dialog box. Profiler & Optimizer
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4.

q
Step-by-Step Rotation: this area lets you define the rotation angle in degrees. clockwise) around the X axis whereas clicking -X will rotate the light source by the specified angle negative (i. When the rotation angle has been defined. click the desired button to start rotating your light source around the corresponding axis by the angle you specified. The default value is 10. the light source is updated simultaneously in the geometry area. Y and Z directions.e.
q
Direction: the three spin boxes displayed let you define the position of the direction vector along the X.
For instance. As soon as you modify a value.00 but you can enter your own value if needed using the spin box.FreeStyle Shaper. The direction vector represents the privileged direction of illumination of the source and is visualized by the red arrow whose origin is the light source origin. the rotation step as well as the quick orientation. Profiler & Optimizer
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Edit Light Direction
This dialog box lets you edit the light direction.e. anticlockwise) around the X axis:
. clicking X+ means that the light source will be rotated by the specified angle positive (i.

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Quick Orientation: this area lets you position the light source parallel to the absolute axis system.
For detailed information on this dialog box. click OK to validate your parameters. Profiler & Optimizer
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Starting position: X
New position: X+ Rotation = 45 degrees
Note that using these buttons amounts to manipulating the light source directly in the geometry area using the Ctrl key. refer to Adjusting Light Source Parameters in the Real Time Rendering documentation. Diffuse. and Specular. For instance. clicking -Y will invert the position of the light source along the Y axis:
q
Compass: this button lets you position the light source according to the compass orientation. clicking Y will modify the light origin in order to position the light source parallel to the Y axis.
Edit Light Parameters
This dialog box lets you modify the intensity of a light source is the maximal lightness value of three colors: Ambient.
When satisfied.
. Inversely.FreeStyle Shaper.

If you want to use afterwards one of the light positions you saved.
Once you are satisfied with the position of your light source. you will be able to rotate up or down your light source around the X axis only if you activate the Rotate around Y command. When finished. You can save as many positions as necessary but keep in mind that you are not allowed to modify the position name. Y or Z axis using the two green manipulators
q
if you activate the Rotate around X command. for instance "Direction. Y or Z axis. you will be able to rotate up or down your light source around the Y axis only if you activate the Rotate around Z command. the Free Rotation contextual command is activated and lets you rotate freely your light source around the X.FreeStyle Shaper.
Rotation
The rotation commands let you rotate the light source around the absolute axis system:
q
by default. "n" being incremented by one for each new position you save. click the Save button to store the light position.n. just re-select the Save Light Direction contextual command then double-click the desired position: the light position will be updated accordingly in the geometry area. click OK to validate. you will be able to rotate up or down your light source around the Z axis only.1" for the first position. Each light position is saved under the following name: Direction. Profiler & Optimizer
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Save Light Direction
This dialog box lets you save the light source position. the green manipulators are hidden and only the light target is displayed:
.
q
q
When you select the rotation around the X.

This command applies to the local X and Y axes of the light source. you can also click anywhere in the geometry area then press the space bar to hide the manipulator symbol. one manipulator is locked
. This is illustrated by the example below in three steps (from left to right): 1. you can also lock the selected manipulator using the Lock Manipulator contextual command.FreeStyle Shaper. Locking a manipulator means that the rotation in the plane defined by the selected manipulator will be locked: the locked manipulator is hidden and you will only be able to move your light source around the unlocked axis of the light source which means that the mouse will move only up or down. the cursor shape changes) without being bothered by the display of this manipulator on your model. Profiler & Optimizer
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Lock Manipulator
When you point at one of the two green manipulators then right-click. This is especially useful when working with big models because you can still change the light position by pointing at the hidden manipulator (in that case.
Once a manipulator is locked.

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3. you can still drag the hidden manipulator to modify the light direction
To redisplay the manipulator. you just need to press the space bar again.
.

These tools are available from the FreeStyle Dashboard. Display orders along U or V: select the element and click the icon to display the order number along U and/or V Display control points temporarily: click the icon to display control points on selected elements while another command is running. Display continuities on an element: select the element and click the icon to display a text indicating the continuity type on the element. Create a temporary analysis: select this mode once you enter a command in order to get a feedback on the connection quality. Insert in a new geometrical set: select this mode once you enter a command to create the result of the operation in a new geometrical set.FreeStyle Shaper. Display contact points on an element: select the element and click the icon to display the contact points and their manipulators on the element. The operation is performed on a copy of the original element. Profiler & Optimizer
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Generic Tools
This chapter deals with generic tools available in FreeStyle Shaper. Attenuate displacement: choose the attenuation value for the manipulators' step.
. Keep the initial element: click the icon and use another command do create/modify an element. Display the tension on an element: select the element and click the icon to display the tension vector and value on the element.
Generic Tools
Display dress-up options: set the display options then apply or remove the visualization options on selected elements. Auto-detection: specify the search type and set the auto-detection parameters. the Generic Tools and the Selection toolbars and the Tools menu bar:
FreeStyle Dashboard
Create datums: click the icon to deactivate the History mode.

Tools
Analyze using parameterization: select the Tools -> Parameterization Analysis. and a mirror plane.
User Selection Filter
Select using a filter: select an object. a curve. Manipulate Views: click this icon to move backward in the viewpoints.. Define Views: click this icon to reverse the viewpoint. Profiler & Optimizer
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Display information on elements: click the icon and select any element. Define views: drag and drop the compass and click the icon to define the viewpoint.FreeStyle Shaper. Manipulate Views: click this icon to move forward in the viewpoints. and use the Selection Filter toolbar to manage element types and modes. Define an axis system: click the icon. or a surface and right-click the pictographic tag to choose the support. command and define a filter for your query.
. Manage the compass: click the adequate icon in the displayed toolbar to define the compass orientation. and enter coordinates or select geometry to define the three axes. Work with a 3D support: click this icon and select a define the 3D support type: Reference or Local
View Manipulation
Stretch view analysis tool: set the stretching ratio. Display a part symmetrically: select a part..
Miscellaneous
Select a support: select a point. Manipulate views: click the adequate icon to freeze viewpoint manipulations.

select Edit and/or Keep this point from the contextual menu. click OK. Select using multi-output: select several elements. grouping elements.FreeStyle Shaper. The Multi Output feature appears in the specification tree. Select using multi-selection: select one or more elements through the Tools Palette and validate you modification to return to the current command.
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Edit and keep a point: right-click a point.

the Datum mode is permanent.FreeStyle Shaper. there are no links to the other entities that were used to create that element. Profiler & Optimizer
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Creating Datums
This task shows how to create geometry with the History mode deactivated.
It will remain deactivated until you click on the icon again. Click the Create Datum icon to deactivate the History mode.
. A click on the icon activates the Datum mode for the current or the next command. 1.
The History mode (active or inactive) will remain fixed from one session to another: it is in fact a setting. when you create an element. In this case. You only have to click again the icon to deactivate the mode. If you double-click this icon.

in fact. 1. The offset surface is automatically visualized as a meshed surface.
. Click the Keep Original icon
from the FreeStyle Dashboard.
2.CATPart document containing FreeStyle elements. Profiler & Optimizer
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Keeping the Initial Element
This task shows you how to retain an element on which you are performing an operation. Open the Offset1.FreeStyle Shaper.CATPart document. Select a surface and click the Offset icon for example.
The Offset dialog box is displayed. you are working on a copy of the initial element. as soon as you perform an action in which you create or modify geometry. When this command is active. or any .

. The initial element remains unchanged and a new element is created. providing it was active while performing the command (and vice-versa).FreeStyle Shaper. the initial element would have been replaced by the newly created element. Profiler & Optimizer
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3. Click OK in the current command. Had you not clicked on the Keep Original icon . The Keep original icon remains active once you click OK.

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Inserting in a New Geometrical Set
This task shows how to insert the result of an operation in a new geometrical set. 5. Select the cutting curve(s). 6. 2. 4. and Dress-Up commands. Let's take an example with the Break Surface command. The FreeStyle Break dialog box displays.
3. Disassemble. It is only available with the Break (Curve and Surface). Open the Break1. Choose the Surfaces by curves break type. Copy Geometric Parameters. Select the surface to be cut.
. Click the Break icon . Click OK.FreeStyle Shaper. 1. Click the Insert in a new geometrical set icon in the
FreeStyle Dashboard.

For further information about the Break command.FreeStyle Shaper. Profiler & Optimizer
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All the created surfaces resulting from the break are displayed in a new geometrical set in the specification tree. please refer to the following chapters: Redefining Surfaces Limits and Trimming Curves.
.

Select the points. we chose the Porcupine Curvature Analysis. In our example. Click the Temporary Analysis mode icon in the FreeStyle Dashboard. 1. Select the analysis of your choice in the Shape Analysis toolbar. 4. Profiler & Optimizer
Creating a Temporary Analysis
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This task shows how to create a temporary analysis during the creation process of a feature. 2. The 3D curve dialog box is displayed.
5. Click the 3D Curve icon . Net and Sweep commands. Fill.
.CATPart document.
3. This command is only available with the 3D curve. Choose the Through points type.FreeStyle Shaper. Let's take an example with the 3D curve command. Open a new .

q
.
q
You can perform several analyses while in the Temporary Analysis command: all of them will appear in the specification tree under the Free Form Analysis node. 7. a persistent FreeStyle analysis will be performed. you can perform a Connect Checker or a Distance analysis: the surface to be analyzed is automatically selected. Thus when you click OK in the 3D curve dialog box to create the curve. Click OK in the Curvature Analysis dialog box. Profiler & Optimizer
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6.
You must activate the temporary analysis mode before running any analysis. the Temporary Analysis node disappears from the specification tree. The temporary analysis is updated accordingly.FreeStyle Shaper.1) appears below.
The analysis is not persistent. Once you exit the creation command. Net or Sweep command. the analysis disappears. The Temporary Analysis node is displayed in the specification tree and the associated analysis (here Curvature Analysis. While in the Fill. Select another point in the 3D curve command. as well as all surfaces that share at least one border with it. Otherwise.

Choose one of the four detection types from the FreeStyle Dashboard:
q
Click the Snap On Vertex icon element. Move the pointer close to the geometric element you wish to snap to. to define the local axis-system.
q
When checking the Search Dressing option from the Tools -> Options -> Shape -> FreeStyle tab. This is also useful to position the compass at a specific location on an element. border. and the Snap On Cpt icon the system automatically displays the control points on the geometry detected below the pointer. Click the Snap On Cpt icon selected element. provided a command is running.
1.FreeStyle Shaper. Click the Snap On Segment icon selected element
to detect the closest corner of the selected
q
to detect the closest border (edge) of the
q
to detect the closest control point on the
q
to detect the the closest segment of the
2. The specified element (corner. control point or segment) is automatically detected and selected. Click the Snap On Edge icon selected element.
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Auto-detection
The Auto-detection tool enable you to perform a remote point selection which is especially useful for selecting on the fly point on geometry.

to another element.
. the auto-detection still is available.
q
Use the Shift key to activate/deactivate temporarily the auto-detection capability on the point you are currently trying to snap. or not. but the control points are not displayed.FreeStyle Shaper. yet the Snap On Cpt option is active. Profiler & Optimizer
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If this Search Dressing option has not been checked.

This attenuation factor is saved in the application's settings. 1.
. The attenuation lets you define the ratio between the mouse displacement and the actual displacement of the manipulator in the geometry. Profiler & Optimizer
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Setting the Manipulators Attenuation Factor
This task shows you how to set the attenuation value for the manipulator's displacement. Open any .FreeStyle Shaper. and is defined in the FreeStyle Settings.CATPart document containing FreeStyle elements. Choose one of the four attenuation ratio from the FreeStyle Dashboard:
q
Click the No Attenuation icon
to use the attenuation value as set in the
FreeStyle General Settings (default value) Click the Slow icon Click the Medium icon Click the High icon to use the square default attenuation value to use the cubic default attenuation value to use the 104 default attenuation value
q
q
q
Each attenuation value equals the previous value (in the dashboard) multiplied by the default value.

Once they are displayed. 3. Three types of manipulators can be displayed on a given element. 2.
. 1. or by checking the adequate option in Tools -> Options -> Shape -> FreeStyle.CATPart document. 4. Click the Match Surface icon Matching Surfaces).
Texts indicating the continuity type wherever available are displayed. continuity contact points tension (P2 only) U and V orders
These manipulators are displayed either by using the Dashboard (P2 only) as illustrated in this task. and select the two edges to be matched (see
2. Click the Continuity icon from
the Dashboard. whether the selected or the resulting element: 1.
Displaying Continuity
Open the MatchSurface1.FreeStyle Shaper. their behavior is identical regardless of the chosen interface style. Profiler & Optimizer
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Displaying Manipulators On Elements
This task shows you how to display manipulators on elements and how to modify their values.

Right-click on a text to display the contextual menu.
.
Displaying Contact Points
Open the BlendSurface1. or modify the geometry itself. A forbidden sign may even be displayed and the system will prevent you from modifying the element in a specific direction. if it does not make sense geometrically speaking. Profiler & Optimizer
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3. Click as many times as needed to go down to the desired continuity type.FreeStyle Shaper. The text changes to Curvature and the elements are updated in accordance.
In some cases the chosen type of continuity is not compatible with the geometry or the modification.
You can also simply click the text. a warning is displayed directly onto the geometry at the location where the inconsistency arises. and choose the Curvature continuity item. You can then change the continuity. It will automatically change to the next type. Shift-clicking goes up in the list. In that case.CATPart document.

and select an edge on each surface.FreeStyle Shaper. Click the Blend Surface icon . allowing you to interactively define the blend limits by simply sliding them along the boundaries. Click the Contact Points icon from the dashboard.
The blend surface is computed.
Manipulators are displayed on the connection. Profiler & Optimizer
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1.
.
2.

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You can edit the contact points by right-clicking any of them to display the contextual menu and choosing the Edit item. Click the Tensions icon from the Dashboard.
Green segments representing the direction and limits tension are
. The Tuner dialog box opens to let you key in a new value.
1.
. in percentage of the total boundary.
2.
Displaying Tensions (P2 only)
Open the BlendCurve1.CATPart document. Select two curves and click the Blend Curve icon The blend curve is previewed.

or invert the tension direction.CATPart document. Profiler & Optimizer
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displayed. Click the Match Surface icon Matching Surfaces). V Orders
Open the MatchSurface1. You can modify the tension by sliding the displayed value along the green segment.FreeStyle Shaper.
Displaying U. and select the two edges to be matched (see
.
You can also edit the value. 1. using the contextual menu on the value.

. Click the U. Profiler & Optimizer
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2.
Numbers are displayed on the geometry.
3. V Orders icon from the Dashboard. It will automatically change to the next digit down the list.FreeStyle Shaper. indicating the order number of the element along the U and V directions. Shift-clicking goes up in the list. Right-click on a text to choose another order value
You can also simply click the text.

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The Automatic option enables you to modify the order and the segmentation of the matching surface so that the continuity is respected.
.FreeStyle Shaper.
The surface order is instantly modified. but you will see it only when using the Control Points icon for example:
For curves. only the order along U is displayed.

.CATPart document containing FreeStyle elements.CATPart document. if there were two curves to be projected for example when using the Project Curve icon the control points are displayed on all the resulting elements. Profiler & Optimizer
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Displaying Control Points Temporarily
This task shows you how to temporarily display control points geometry while in a FreeStyle command. Successively select two curves.
Control points are displayed in blue on the matched curve. from the
3. or any .
4. Click the Match Curve icon . 1.FreeStyle Shaper. the control points are removed as opposed to those displayed using the permanent visualization options (see Setting FreeStyle Visualization Options). Check the Control Points option in the Display area of the Tools -> Options -> Shape -> FreeStyle -> General tab or click the Furtive Display icon Dashboard (P2 only).
Multi-selection is available. meaning that if several elements are involved in the current command. The first curve is automatically modified so as to be connected to the second curve. Open the MatchCurve1. Once you exit this command. Click OK in the current command. 2.

Click the Apply Dress-Up icon . or not. Open the VisuOptions1.FreeStyle Shaper. Profiler & Optimizer
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Setting FreeStyle Visualization Options
This task shows you how to display or hide permanent control points and curve/surface segments on FreeStyle Shaper elements for analyses purposes. segments. or not.
The Dress-Up Options dialog box is displayed.
3. control points
q
the control points type to display.CATPart document. Select the element on which you wish to display the control points.CATPart document containing FreeStyle elements. Set the type of visualization you want to apply to geometric elements.
q
The Isoparametrics by patch is inactive but provides information on the number of isoparametric curves (dotted lines) per surface patch (delimited by solid lines). 1.
. You can choose:
q
to display. or any .
2.

Contextual options
a.
5. then click Apply. When selecting an arc limit of a curve: It enables you to either keep the arc limit you right-clicked or all the arc's limits. uncheck the Control Points.
q
Keep this arc limit: a 3D point appears in datum mode in the specification tree Keep all arc's limits: all the 3D points used to create the 3D curve appear in datum mode in the specification tree
q
. The control points and mesh lines are displayed on the selected element. Activate the Segmentation option. Click Apply.FreeStyle Shaper. Profiler & Optimizer
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4.

q
. meaning that you can apply different options to several elements. If you wish to create the 3D points or curves in a new geometrical set instead of the current geometrical set. As the 3D points and curves are created in a private body. its content cannot be modified: you cannot delete or add elements. Therefore patches limits do not necessarily correspond to surfaces limits (in the case of trimmed surfaces for instance). The visualization options are as defined by the user and remain on the selected elements till you click the Remove Visualization Options icon them using the Dress-Up Options dialog box again. Profiler & Optimizer
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b. or till you modify
Multi-selection applies with these display capabilities:
. As long as the icon is active. Click OK. When selecting the patches limits of a surface:
q
Keep all patches limits: all the 3D curves used to create the patch limit appear in datum mode in the specification tree. The control points type is applied globally to the document. but if you save. 6. the options defined last will be applied to all the elements on which visualization options have been set. close then open the document again.
Note: only patches limits are created.FreeStyle Shaper. as opposed to using the Control Points icon as described in Editing Surfaces Using Control Points or Editing Curves Using Control Points. click the Insert In a New Geometrical Set icon from the FreeStyle Dashboard. a new geometrical set is created each time you run the Dress-Up command. q No modification is possible on the control points.

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Capabilities available from the FreeStyle Dashboard are datum creation and insert in a new geometrical set.

planes.
The Geometric Analysis dialog box is displayed. Open the GeometricInformation1.) whether the element has been trimmed. or surface. such as:
q
the element type (Nurbs surface or curve. or taking part in the composition of another element (intersection curve.
2. and so forth).CATPart document containing geometrical elements. a vector representing the element's orientation (U for a curve. face of a pad. Pline.CATPart document. are not analyzed. cylinder axis. such as any curve. either as a stand-alone element. for example. and U & V for a surface) is displayed on the geometrical element itself.
. Moreover. or any . or not the number of segments (components) in both U & V direction (where applicable) the order of the element in both U & V direction (where applicable)
q
q
q
is displayed in the dialog box.FreeStyle Shaper. therefore elements such as Cloud of points. Click the Geometric Information icon . 1. Select the element for which you want to display information either in the geometric area or in the specification tree.
Information. etc. Only geometry of topological cells is analyzed. Profiler & Optimizer
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Displaying Geometric Information On Elements
This task shows you how to display or hide geometric information on geometrical elements.

you are back into the initial command. The current command is frozen.
to exit the command. the maximum order is 6.
q
You can stack this command on top of the current command. be composed of more than one cell) and the system cannot determine which element is to be analyzed. i.e. and when you exit the information command. that you editing an element using its control points. or simply click
q
You cannot select an element from the specification tree as the selected element might be too complex (i.
q
Uncheck the Geometric Information icon another icon. Profiler & Optimizer
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In the case of a 3D curve created using the Control Points type.e.
The geometry type is categorized as follows:
Displayed Type NupbsCurve NupbsSurface NurbsCurve NurbsSurface PNupbs PNurbs PSpline PLine Line Plane Cylinder Helix FilletSurface
What is it ? Non Uniform polynomial B-Spline Curve Non Uniform polynomial B-Spline Surface Non Uniform Rational B-Spline Curve Non Uniform Rational B-Spline Surface Parametric non rational curve on a surface Rational parametric curve Parametric curve on a surface Isoparametric curve on a surface Line or line segment Plane or planar face Cylinder Helix Procedural Fillet surface
. you can activate the Geometric Information icon.FreeStyle Shaper.

. for example. The Part5. 1.FreeStyle Shaper. 4.
3. and so forth). but to view the final element as a whole. Select the mirror plane. Click the Visual Symmetry icon. It can be a plane or any planar face that the system recognizes as a plane (a planar face of a pad. Profiler & Optimizer
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Displaying a Part Symmetrically
This task shows you how to visualize a part symmetrically in relation to a plane. in a product context. then double-click it. Expand the tree down to the Part5. therefore with a smaller document size-wise.CATProduct document. Select the Part to be mirrored from the specification tree.CATPart now can be edited within the FreeStyle Shaper workbench. Open the Product_to_symmetrize. 2. This allows you to work on half of the geometry only.

even though it will be saved within the document.
.
The part is also duplicated in the specification tree. It is modified only as the result of modifications performed on the initial part: Indeed you are not even allowed to select the mirrored elements in the geometry. If you select a mirrored element in the specification tree. However. you will note that the highlighted geometry belongs to the initial part. this part cannot be edited as geometry. Profiler & Optimizer
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A part. symmetrical in relation to the selected plane.FreeStyle Shaper. is displayed.

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5. Choose the adequate options and modify the initial part as needed. Click the Control Points icon .
You can then save and close the .
7.CATProduct documents.
.
6. Click OK in the Control Points dialog box.FreeStyle Shaper. and is present when you open these documents again.
The mirrored part reflects exactly the modifications imposed on the initial part.
The Control Points dialog box is displayed.CATPart and . The mirrored part is retained.

.
q
Click the Reset Compass to XYZ icon
or press F7 to reset the compass parallel to
the main axes (X.FreeStyle Shaper. Y and Z) of the model.
q
Click the Most Seen Plane icon mode. Y and Z otherwise U.
If the compass is "in" the main axes of the model. V and W. The origin is kept in the model until the toolbar remains open.
q
Click the In Model or on Perch icon
to switch the compass from the perch to the
model or vice versa.
to activate and deactivate the Most Seen Plane
q
Click the Set Compass Orientation icon
or press F6 to orientate the compass by
selecting either an existing plane or three points (via the Autodetection command). Here are summarized the main features of its eight icons:
q
. Flip to VW or YZ
or Flip to WU or XZ
icon to
switch the compass base to the three planes of its trihedron. Create a planar surface. The point selection is based on Autodetection parameters. Press F5 or click the Quick Compass Orientation icon The Quick compass orientation toolbar is displayed. the icons indicate X. Please refer to the chapter called Editing Curves Using Control Points documentation to orientate the compass using control points.
Click the Flip to UV or XY
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Managing the Compass
This task shows you how to quickly manage the compass orientation. This option is not active when the compass is already set according to the axes.

The Quick compass orientation toolbar remains active until you close it by clicking the cross in the upper-right corner or. . Flip to VW or YZ or Flip to
. if you have activated it with the icon. F6. the toolbar is displayed and the shortcuts are effective from then on. By default. that is
to create a plane corresponding to the compass basis.FreeStyle Shaper. Profiler & Optimizer
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q
Click the Create Compass Plane icon
or press F8 to drop the compass plane.
These four shortcuts (F5. This icon is activated only when the compass is in the model. by clicking the icon again. Therefore when you first hit one of the keys. F7 and F8) are effective only when the Quick compass orientation toolbar is displayed. elements are created in the current active plane as defined using the Current plane orientation toolbar containing the Flip to UV or XY WU or XZ icons.

1.
An axis system is composed of an origin point and three orthogonal axes. Select the Insert -> Axis System command or click the Axis System icon .FreeStyle Shaper.
.
Open the PowerCopyStart1. There are two ways of defining it: either by selecting geometry or by entering coordinates. It can be right or left-handed. Profiler & Optimizer
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Defining an Axis System
This task explains how to define a new three-axis system locally. You can choose from different types of axis system:
q
Standard: defined by a point of origin and three orthogonal directions (by default the current directions of the compass)
Here only the point was selected and nothing specified for the axes. This information is displayed within the Axis System Definition dialog box.
The Axis System Definition dialog box is displayed.CATPart document.

and Z directions
Here. the Angle 2 and Angle 3 were set to 30 degrees.FreeStyle Shaper. The axis system looks like this:
. Both computed axes are then parallel to those of the current system. Profiler & Optimizer
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q
Axis rotation: defined as a standard axis system and a angle computed from a selected reference
Here the Y axis was set to the standard axis system Y axis. The application then computes the remaining coordinates. and a 15 degrees angle was set in relation to an edge parallel to the X axis.
q
Euler angles: defined by three angle values computed from the initial X.
2. Y. Select the point as shown to position the origin of the axis system you wish to create.

for instance click the X axis field and select a line to define a new direction for x axis. and Planes.FreeStyle Shaper. If you are not satisfied with x axis. using the Create Line contextual menu on the selection field.
. Similarly you can create Points. and selecting two surface vertices. You can also select the Rotation contextual menu. for example.
q
4.
q
It can be a line created along the surface edge. and enter an angle value in the X Axis Rotation dialog box. Checking the Reverse button next to the Y Axis field reverses its direction too. Profiler & Optimizer
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3. The x axis becomes colinear with this line. Click the y axis in the geometry to reverse it.

retain the Y and Z coordinates. Profiler & Optimizer
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5. the application detects if its axes are orthogonal or not. Key in X = -1. Click More to display the More. Inconsistencies are revealed via the Update diagnosis dialog box. 6..
As you are defining your axis system. and click Close.FreeStyle Shaper. The Z Axis dialog box appears. Right-click the Z Axis field and select the Coordinates contextual command. The axis system is modified accordingly.. The coordinates of Y and Z axis are displayed in the third and fourth row respectively. The coordinates of X axis are displayed in the second row. and is now left-handed.
The first rows contains the coordinates of the origin point. You can also define axes through coordinates.
7. dialog box.
.

The absolute axis at the bottom right of the document then becomes the current axis system.
9.
Editing an Axis System
You can edit your axis system by double-clicking it and entering new values in the dialog box that appears.1 is now current. it is highlighted as shown aside. to define a sketch plane for example. If you wish to constrain them. It is displayed in the specification tree. You can also use the compass to edit your axis system. Click OK. Local axes are fixed. When it is set as current.1 from the specification tree and select the Axis System. The axis system is created. The display mode of the axes is different depending on whether the three-axis system is righthanded or left-handed and current or not.:redefines the axis system Isolate: sets the axis system apart from the geometry Set as Current/Set as not Current: defines whether the axis system is the reference or not. Uncheck the Current option if you do not want to set your axis as the reference. you need to isolate them (using Isolate contextual command) before setting constraints otherwise you would obtain over-constrained systems.FreeStyle Shaper.
q
q
q
..X object in the specification tree lets you access the following contextual commands: Definition.1 object -> Set as current contextual command. You can then select one of its plane.. Note also that editing the geometrical elements selected for defining the axes or the origin point affects the definition of the axis system accordingly. Profiler & Optimizer
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8.
THREE-AXIS SYSTEM
right-handed right-handed left-handed left-handed
CURRENT
yes no yes no
AXIS DISPLAY MODE
solid dashed dotted dot-dashed
Right-click Axis System. Right-clicking Axis System. Axis System.

q
. It is composed of three regular grid of lines. that aggregates 3 selectable work on supports. Open the WorkOnSupport1. It allows you to create reference points on the fly on each support. This task shows how to create a 3D support. These features do not appear neither in the specification tree nor in the 3D geometry but are aggregated under the feature using them. Click the Work on Support 3D icon . The three directions of the main axis system define the grids directions. Grids are used both as an input to create geometry as well as visual help.CATPart document. Note that you can modify these values at creation. not at edition.FreeStyle Shaper. edges). and that there can only be one value per grid. You will no longer have to explicitly select the support element. Profiler & Optimizer
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Working with a 3D Support
This command is only available with the Automotive BiW Template product. generally set on the three main planes of the part. The Work on Support 3D dialog box appears.
q
Each of three grid lines has one default primary spacing of 100mm for each direction. 1. It also allows you to create sub-elements of the grid on the fly (points. You can edit the spacing values by clicking on the spacing tag to edit and modify them. whenever you need a reference point to create other geometric elements. You can also modify the name of the labels of the main directions by clicking on the direction tag.

Click OK in the dialog box. Profiler & Optimizer
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Labels' directions and primary spacing are defined in Tools -> Options -> Shape -> Generative Shape Design. Please refer to the Customizing section of the Generative Shape Design documentation for further information. Choose the Labels position:
r
Full screen: labels are displayed all around the screen Bottom/Left: labels are displayed on the bottom left of the screen None: no label is displayed
r
r
3. There can be only one reference 3D work on support. There can be as many local 3D works on support as desired.
4.
r
Local: a local axis system must be specified.
. Define the Support Type:
r
Reference: the 3D support is created according to the main axis system. The elements (identified as Working support 3D. 2. Here is an example with a reference and a local 3D work on support.xxx) are added to the specification tree under the Working supports node.FreeStyle Shaper.

FreeStyle Shaper. the 3D work on support is no longer parallel to the screen.
icon from the
The active work on support is visualized and labels are displayed on each straight line.
Note:
q
There can only be one active 3D work on support at the same time. Select the Top View Quick View toolbar.
q
q
By default the last created working support is displayed in red in the specification tree. Use the Set As Current/Set As Not Current contextual menu on the working support features.
q
If you move the compass.
. You can also set the axis system as not current to reactivate the three planes and define the reference 3D support as the current support. Profiler & Optimizer
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5.
q
The work on support must be parallel to one of the three planes to be visualized. all related features are updated. When the local axis system is modified. the active 3D work on support may be seen independently in each view of the same document. As a consequence. or the Working Supports Activity icon to define which is the default current support that will be automatically selected when entering a command that requires a working support.

updated. Click the Snap to point icon intersection point on the grid. As a result. to snap the point being created onto the nearest
q
q
q
. or deleted just as any other feature. The created points using a support are aggregated under the parent command that created them and put in no show in the specification tree. you can directly click onto the support to create points. Once you choose to work on the 3D support. line. therefore allowing you to use them more easily.FreeStyle Shaper. This capability is available with commands such as point. and most commands where you need to select points as inputs. Each 3D working support can be edited. the retrieved features are selected in the current editor and highlighted in the specification tree. Profiler & Optimizer
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Use the Get Features on Support contextual menu on the working support features to retrieve the features created from a single or a multi-selection works on support.

The control points are grayed out. the geometry looks like this:
With a value of 1.
2.5. It is especially useful to examine precisely the curvature of an element from different viewpoints and with specific angles.CATPart document. and the Stretch View dialog box is displayed:
3. meaning you cannot use them for geometry modifications. we choose to open two windows (Window -> New Window) and to display them horizontally (Window > Tile Horizontally). This task shows how to use the stretch view tool prior while analyzing a FreeStyle element. 1. Click the Stretch View icon
. Profiler & Optimizer
Using the Stretch View Analysis Tool
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This command is only available with the FreeStyle Optimizer. The Control Points dialog box is displayed.
With a value of 0. Stretching means distorting the space view.5. To make it more explicit. Select a surface and click to display the control
points on the surface in both windows. without affecting the element itself. This stretching is done according to a ratio between the Y and X axes (Y/X) taking the screen as a reference into the active window. Modify the value in the Stretch View dialog box. the geometry looks like this:
.FreeStyle Shaper. Open the Stretch1.

Click Reset.
The resulting stretch looks like this:
. Profiler & Optimizer
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4. The center of the trap (cross) becomes the center of the screen.
You could also stretch a specific area of the screen. The default value is taken into account (1.00).FreeStyle Shaper. using a trap. Using the Ctrl-key. the trap center will be located where you click first. The view no longer is stretched.

move elements and so forth. the views remains. and you can continue to deform the surface as you wish. using the control points. You can rotate. For example. you can continue to use any other FreeStyle Shaper or Optimizer capability. you could apply the Curvature analysis. Profiler & Optimizer
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5.
q
Whatever the stretch options you choose. you can still manipulate the geometric elements as usual.
Curvature analysis with no stretch
Stretched curvature analysis Even though the stretch is performed in reference to your screen (X is the horizontal axis and Y the vertical one).FreeStyle Shaper.
q
. Click Close.

used to define the 3D viewpoint. in order to set a specific viewpoint. is active. By default. In this mode.CATPart document. 4. 3. and drag to rotate freely in space. the four main manipulations. translation zoom (in or out) rotation focusing on a specific point (double-click on mouse key 2). are
Open the ManipulateViews1. the Standard View Manipulation available.
1.FreeStyle Shaper. Press and hold key 2 then 1 of the mouse. 1. Profiler & Optimizer
Manipulating Views
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This command is only available with the FreeStyle Optimizer. When opening the document. 2. you should see something like this:
This task shows you how to constrain views.
.

The tuning defines the movement amplitude. simply click backward or to move forward in the viewpoints.
This attenuation step definition is also affected by the Tuning value defined in the general
5. using the right and left arrows
r
q
Similarly.
4. movement will seem slower. you can zoom in and out. you can now only rotate about the Z screen axis. use keyboard shortcuts to manipulate views according to pre-set steps: r 90° around the Z screen axis. you may wish to come back to a preceding viewpoint. Display the whole Manipulating Mode toolbar (under the
icon).
q
q
Still holding down mouse keys 1 and 2. If you click the Zoom And Translate
icon. to move
q
If you define a manipulation mode in a multi-view configuration and you switch to another view. When changing viewpoints. you are able to zoom as usual. using the right and left arrows.
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2.
Still holding both mouse keys. the selected mode is no longer active. Simply click the Standard View Manipulation icon to reset the default options.
3. This is especially useful when working in Stretch view mode. Similarly you can click the Rotation About X Screen Axis
or Rotation About Y Screen Axis
icon to rotate around
the screen X or Y axis respectively. To do this. but still hold key 2. Click the Rotation About Z Screen Axis
icon.FreeStyle Shaper. To redefine the tuning.
No rotation whatsoever is allowed. using the Up/Down keys
r
90° around the X screen axis. using the up and down arrows 90° around the Y screen axis. i. if you decrease the value.
.
If you release key 1.e. refer to the FreeStyle settings and the Setting the Manipulators Attenuation Factor chapters.

4.
1. that you want to see. Click again if you want to reverse it again. at the point where you dropped that compass. Drag the compass onto the exact point of
geometry.
2. Click the Reverse Viewpoint
icon. You now can see the geometry from under the compass.
Open the ManipulateViews1. using the compass on the geometry.CATPart document.
.
3. The viewpoint changes immediately. This also defines the viewing direction. at the point where you dropped that compass. Click the Interactive Viewpoint Definition
icon.FreeStyle Shaper.
The viewpoint changes immediately. Profiler & Optimizer
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Defining Views
This command is only available with the FreeStyle Optimizer. You now watch the geometry from above the compass. This task shows you how to rapidly define a viewpoint.

to move backward or to move forward in the To do this.FreeStyle Shaper. Profiler & Optimizer
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When changing viewpoints.
. simply click viewpoints. you may wish to come back to a preceding viewpoint.

. for example. Select Tools -> Parameterization Analysis. This is particularly useful when managing power copies. Use the Filter combo and choose to display Root Features.
2.FreeStyle Shaper.
The query is launched and the viewer automatically updates. Profiler & Optimizer
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Analyzing Using Parameterization
This task enables to analyze the CATPart structure and shows how to isolate specific features within a part.
..CATPart document. 1. Open the Parameterization1.
The Parameterization Analysis dialog box opens.

FreeStyle Shaper. if you want to display deactivated features only. select the Isolated Features filter to display both deactivated and datum features. Profiler & Optimizer
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Deactivated features as well as datum features are displayed. Available filters are: r All Sketches
r
q
Over-constrained sketches Fully-constrained sketches Under-constrained sketches Inconsistent sketches External references Inactivated features Root features Leaf features Isolated features
r
r
r
r
r
r
r
r
. However. for example. or use the contextual menu to reframe on or display its properties. Click the Display Body Structure icon to
display the graph keeping the tree structure.
q
Features displayed in the viewer can be used in the same way as in the specification tree: double-click a feature to edit it. The viewer can still be open while performing other operations. Similarly. select the Inactivated Features filter.
Each feature is displayed within its own body.
3.

refer to the Analyzing and Resolving OverConstrained or Inconsistent Sketches chapter in the Sketcher documentation. and Checks Bodies
r
r
r
r
r
For further information about sketches. refer to the Isolating Geometric Elements chapter. For further information about Isolated features. For further information about Features with stop update and active stop update. refer to the Part Design documentation. Rules.FreeStyle Shaper. For further information about Bodies.
. refer to the Updating Your Design chapter. Profiler & Optimizer
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Features in error Waiting for update features Features with stop update Features with active stop update Knowledge formulas. refer to the Knowledge Advisor documentation. For further information about knowledge formulas.

or a curve resulting from an intersection. Profiler & Optimizer
Selecting a Support
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This task shows you how to select a support in the case several supports are detected.
. and the Blend Surface dialog box is displayed. the number of generated faces will be equal to the number of joined edges. you can choose the support you need.CATPart document. If a cell of the selected element relies on more than one support.
Creating a blend between a surface and a join
1.
The blend surface is previewed. for example the internal edge of a join.
2. Move the pointer over the edge of a surface and click on it. Click the FreeStyle Blend Surface icon .FreeStyle Shaper. Open the Multi-Supports1. It is available with the following functionalities: q Blend surfaces
q
Match curves Match surfaces Fill Surfaces Net Surface Styling Sweep
q
q
q
q
Let's take two examples using the Blend functionality: q Creating a blend between a surface and a join
q
Creating a blend between two joined entities
In both cases.

Move the pointer over the edge of the second surface and click on it.
7.
8. Right-click the tag to display the number of solutions and choose which support to keep for the blend operation. Move the pointer over the edge of the second surface.
. Click Cancel in the Blend Surface dialog box.
An information tag
is displayed
informing you that two or more surfaces can be selected.1 curve: right-click it in the specification tree and choose Hide/Show from the contextual menu. Hide the Boundary.FreeStyle Shaper.
5.
4. Perform steps 1 and 2 again. Profiler & Optimizer
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3.
The information tag is displayed to inform you that only one surface can be selected for the blend operation.
6.
The blend surface is previewed.

. Move the pointer over a curve and click on it.FreeStyle Shaper.
The blend surface is previewed. Click OK in the Blend Surface dialog box to create the blend surface. and the Blend Surface dialog box is displayed. Move the pointer over the edge of a surface and click on it.
2.
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9.
An information tag
is displayed
informing you that only the selected surface only relies on one support. Click the FreeStyle Blend Surface icon .
Creating a blend between two joined entities
1.
3. Profiler & Optimizer
The blend surface is previewed.

Click the Match Curve icon . Select the second to be matched.2)
You can create a feature whose inputs belong to two different parts. 1. The feature is created in the current part as well. the Blend Surface would have been created between a surface and a 3D curve (and not between Join. Click OK.1 and Join. had you deselected the Feature Element Filter mode. In the above example.
The User Selection Filter toolbar is available with this functionality. Let's take an example with the Match Curve functionality. 2. 4. Profiler & Optimizer
The blend surface is previewed. Click OK in the Blend Surface dialog box to create the blend surface. An import in the current part is performed of the input belonging to the non current part: it is copied in the current part and put in no show.
3.
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4.FreeStyle Shaper.
. Select the first curve to be matched.

The Keep original option must be selected from the FreeStyle Dashboard.FreeStyle Shaper. the matched curve is created in the current part as well as the copied curve which is put in no show.
. Profiler & Optimizer
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In the specification tree.

Choose the Edit item. right-click to display the contextual menu. Profiler & Optimizer
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Editing and Keeping a Point
This task shows you how to edit a point and keep it at its location.
.FreeStyle Shaper. letting you specify the exact position of the point in space and define a step value by which a control point/mesh line moves (Step field).
Checking the Relative option enables you to display the relative mode and specify the relative position of the point depending on its origin as shown in the model. 1. contact point or limit point for example).
2.
The Tuner dialog box is displayed. This option is not available for all functionalities. Move the pointer to a point (control point. Once the value has been defined in the Tuner dialog box. press and hold the Shift key then click one of the manipulator's arrow to move the selected point by the defined step value.

q
.xxx appears in the specification tree.
q
Negative values are allowed. Profiler & Optimizer
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3.FreeStyle Shaper. This contextual menu is available each time manipulators are displayed in the geometry. Choose the Keep this point item to create a point at this location.xxx either on each control point or on the selected control points. A Point. You can create a Point.

: enables you to select elements by drawing a paint stroke
q
q
Any object strictly outside the trap will be selected. Intersecting Trap : enables you to select elements by drawing a trap. and the Shift key to deselect already selected elements. Use the Ctrl key to select several elements.
1. Any object strictly outside or partially outside the trap will be selected.
q
.
q
Any element inside the polygon will be selected. Paint Stroke Trap across them. Choose the selection type:
q
Select
: enables you to select elements or deselect elements in the 3D geometry or
in the specification tree.FreeStyle Shaper. Intersecting Outside Trap Selection : enables you to select elements outside the
q
trap.
q
Elements can either be located inside the trap or be intersected by the trap to be selected. Polygon Trap : enables you to select elements by drawing a closed polygon. Outside Trap Selection : enables you to select elements outside the trap. Control Mode : enables you to validate any selection at once.
q
Elements must be entirely located inside the trap to be selected. Profiler & Optimizer
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Selecting Using Multi-Selection
This capability enables you to perform multi-selection of elements and validate the selection. Selection Trap : enables you to select elements by drawing a trap.

If there are less than one selected element. Finish : enables you to finish and validate the multi-selection.
q
The Tools Palette closes and you go back to definition dialog box. this button is disabled. Profiler & Optimizer
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List of selected items
: enables you to display the dialog box containing the list of
selected items. Multi-selection is available when editing a single feature: double-click it in the specification tree to display the Tools Palette and perform multi-output selection. The number of selected items is displayed in the field to the left of this icon.FreeStyle Shaper.
.

scaling. symmetry. rotation. 5.1 as first element to be Projected. Open the Multi-Output1. Click Close to return to the Projection Definition dialog box. Select as many elements as you need for your projection. 2. Select Translate. The Projected dialog box opens. Click the bag icon the elements list. 1. or 3. affinity and axis to axis Developed wires
q
q
Let's take an example using the Projection and Translation functionalities. Profiler & Optimizer
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Selecting Using Multi-Output
This capability enables to keep the specification of a multi-selection input in a single operation.CATPart document. to display
The number of selected elements is displayed in the
. Click the Projection icon The Projection Definition dialog box appears. 4. as long as the Tools Palette toolbar.
3. Click the Projected field again.FreeStyle Shaper. It is available with the following functionalities: q Intersections
q
Projections All transformations: translation. .

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Projected field. Select Normal as Projection type.1 (Project) in the specification tree. You can create several multi-outputs in the specification tree. Select Extrude. The created elements are aggregated under Multi Output. each one grouping one type of elements.
.
Use the Remove and Replace buttons to modify the elements list.1. 7. all their direct children are selected. Click OK to create the projection elements.FreeStyle Shaper.1 as the Support element.
6.
You can now select one or more geometrical sets and multi-outputs as inputs of the multi-selection. In that case. 8.
The projection is identified as Multi Output.

Shared features are not aggregated under the parent command. To have further information on deactivation. an error message is issued after clicking Preview or OK and displays all features in error. If an element is in error. You are able to manually delete or deactivate the feature(s) in error. When editing the multi-output. Elements can be modified (added. please refer to the Deactivating Features chapter.FreeStyle Shaper. The datum capability is available. only elements that could be generated from the multi-selection are created. the multi-output feature disappears from the 3D geometry and erroneous elements can no longer be generated. Multi-selection is available when editing a single feature: double-click it in the specification tree and click the bag icon to replace it or add new elements.
q
You can deactivate all the elements of a multi-output. you can activate all the elements of a deactivated multi-output. Unshared features are aggregated under the parent command that created them and put in no show in the specification tree. it cannot be created as a datum element. deactivated features are not displayed. As a consequence. Multi-outputs and elements aggregated under a multi-output can be edited separately. simply by double-clicking it in the specification tree.
q
q
q
q
. Profiler & Optimizer
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When one or several features are in error under a multi-output (during creation or edition). or removed): the corresponding multi-output automatically updates. replaced. Similarly.

click Fit then OK. position. if needed select the guiding curve. manipulate the grid to analyze its reflection on the selected surface. if needed. It is used on the same type of elements yet taking the design capabilities one step further. Profiler & Optimizer
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Using the FreeStyle Optimizer
The FreeStyle Optimizer offers complementary capabilities to the FreeStyle Shaper. Analyze reflect curves: Select a surface. Fit a curve to a cloud of points: select the curve to be deformed and the target element. Analyze inflection lines: select a surface. specify the deformation type and use the control points and mesh lines to deform the surface.). specify the fitting parameters and. Fit a surface to a cloud of points: Select the surface to be deformed and the target element. click Fit then OK. viewpoint. if needed. the edge constraints using the contextual menu. specify the fitting parameters and. spacing. set the compass orientation and click the icon to visualize inflection lines
.FreeStyle Shaper. the continuity constraints using the contextual menu. specify the neons grid parameters (number. click Run. Globally deform a surface: Select a set of surfaces.

Here. Profiler & Optimizer
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Fitting a Curve to a Cloud of Points
This command is only available with the FreeStyle Optimizer. Define the fitting parameters in the Fitting area of the Fit to Geometry dialog box.
4. 2. that
. select the cloud of points. Open the FitCurve1.
The Fit To Geometry dialog box is displayed. that is the element to which the curve should fit. and Allowed smoothing have to be taken into account when modifying the curve to fit the existing geometry. Select the target element. 1. You need to specify the Curve tension .FreeStyle Shaper. This task explains how to fit a curve to a cloud of points.
3. Click the Fit to Geometry icon . Select the curve you wish to deform by fitting it to the geometry.CATPart document.

Tangent or Curvature. Point. The curve is modified so as to fit as best the selected geometry. This can be set for each end-point of the initial curve. Profiler & Optimizer
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5. This lets you fine-tune the fit.
.
q
q
Available capabilities from the dashboard are: datum creation. Use the contextual menu on the Free text to impose boundary continuity constraints: Free. once all parameters have been defined. while taking the fitting parameters into account. Click OK in the Fit to Geometry dialog box to accept the new curve as fitted to the cloud of points. You can iterate and click Fit several times. Use the Automatic trap option to reduce the number of points to be taken into account when the target element is a Cloud of Points containing many points.
q
Use the Ctrl key to select several curves to be fitted at a time.
7. Click Fit to accept the definition.FreeStyle Shaper.
6. continuities and orders.

CATPart document.
q
q
. Right-click the Free text on which you want to impose edge constraints. Select the surface. you wish to deform by fitting them to the cloud of points. Profiler & Optimizer
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Fitting a Surface to a Cloud of Points
This command is only available with the FreeStyle Optimizer.
2. A non datum feature cannot be fitted: you must have previously created it using the datum mode or converted it using the Converter Wizard capability.
The Fit To Geometry dialog box is displayed. or set of surfaces. 1. This task explains how to fit a datum surface to a cloud of points. You can choose from four constraint types: q Free: no constraint is imposed on this boundary
q
Point: the resulting surface will still pass through the boundary of the initial surface Tangent: the edge of the resulting surface will be tangent to the initial surface at the selected boundary Curvature: the resulting surface will be continuous in curvature with the initial surface at the selected boundary.
3.FreeStyle Shaper. Open the FitSurface1. Click the Fit to Geometry icon .

FreeStyle Shaper. Use the Automatic trap option to reduce the number of points to be taken into account when the target element is a Cloud of Points containing many points. When the results are satisfying. the surface is projected onto the target geometry. and no longer according to the normals to the initial surface. 7. as shown to the left below. click OK in the Fit to Geometry dialog box. The new surface fits the pre-existing cloud of points.
. You can repeat the operation and deform the surface step-by-step. Click Targets and select the target element in the geometry. Click Fit.
q
Available capabilities from the dashboard are: datum creation. 6.
q
You can also choose to impose a direction when fitting the surface to the cloud of points meaning that the surface will be projected according to cloud of points.
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4. This lets you fine-tune the fit. as shown to the right. continuities and orders.
Using this item you can fit a surface to a cloud of points just as well as you can fit it to any other type of pre-existing geometry.
q
You can iterate and click Fit several times. Define the deformation parameters from the Fit to Geometry dialog box:
q
Tension: indicates which tension coefficient is applied
q
Smoothing: defines the smoothing coefficient to be applied.

CATPart document. Select the surfaces to be deformed. Profiler & Optimizer
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Globally Deforming Surfaces
This command is only available with the FreeStyle Optimizer. Click the Global Deformation icon .
. into which you can specify deformation options: using an intermediate patch or a user-defined axis.
The Global Deformation dialog box appears. using the Control key for multi-selection.FreeStyle Shaper. In this case. This task explains how to deform a set of surfaces in one operation. 1. use the default option: intermediate patch ( Intermediate surface use icon).
2. Open the GlobalDeformation1.

It represents the intermediate surface bounding box. Use the control points and the mesh lines of the planar patch to deform it.
A transparent patch with control points and mesh lines is displayed.
4. All surfaces are automatically and dynamically deformed according to this intermediate patch deformation.
Use it to define the type of operation to be performed on the control points.FreeStyle Shaper. Profiler & Optimizer
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3. q Support defines the type of translation to be applied
q
Law defines the type of deformation that is to be applied when several control points have been selected. The Control Points dialog box is displayed.
. Click Run in the Global Deformation dialog box. The space transformation is defined between the initial patch and the deformed patch.

The Control Points dialog box is displayed. and click the Global Deformation icon .
Open the GlobalDeformation2.CATPart document. Select a guiding surface (here the blue surface). 2. select the surfaces to be deformed.FreeStyle Shaper. you then need to:
1. Use the control points and mesh lines to deform the surface. 3. Profiler & Optimizer
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The final deformed surface looks like this.
q
If you choose the 1 guide option.
. Click Run in the Global Deformation dialog box. Click OK in the Control Points dialog box. The deformation is performed along the selected guide.

it may happen that the set continuities are lost when deforming. surfaces which limits have been redefined. depending on the geometrical configuration. Select two guiding surfaces.FreeStyle Shaper. the top surface is selected as guide. the system globally deforms the surfaces while retaining the continuities on the selected guide. 3. i. Click Run in the Global Deformation dialog box. Click OK in the Control Points dialog box. continuity. and the Continuities on guide is checked. In our example.
q
. auto detection. make sure that you check the continuities between faces. Indeed. and keep original. Profiler & Optimizer
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If you choose the 2 guides option:
1. The deformation is performed along both selected guides.e. attenuation. The Control Points dialog box is displayed. Available capabilities from the dashboard are: datum creation. orders.
q
If you check the Continuities on guide option.
q
When globally deforming re-limited surfaces. 2. Use the control points and mesh lines to deform the surface.

This task explains how to apply reflect curves onto a surface for analysis purposes. Profiler & Optimizer
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Analyzing Reflect Curves
This command is only available with the FreeStyle Optimizer.
The Reflection Lines dialog box is displayed from which you can define a number of parameters:
. Click the Reflection Lines icon The compass automatically is positioned above the surface and a grid of neons is displayed. Each neon is represented by a red line.
.FreeStyle Shaper.CATPart document. Select one or more surface(s).
2. It is an endless neon. 1. Open the Manipulate1. and reflect lines are displayed in red over the surfaces.

when you are using standard viewing manipulators.
3. 4. Profiler & Optimizer
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The number of Neons and the spacing between any two neons. simply click OK in the Reflection dialog box. Reflect lines on the surface evolve as you modify the position of the grid of neons. Once you are satisfied with your analysis. Move the grid using either the standard compass manipulators. clicking one of the grid manipulators rotates the grid by the set value. The position: this option automatically calculates the position of the neon grid (according to the surfaces). In this case.FreeStyle Shaper.
5.
. allowing you to analyze the reflection onto the surface. The viewpoint: r according to the current 3D viewer: reflect lines are re-computed according to the new viewpoint when you are using standard viewing manipulators. Use the Edit angle step contextual menu on the grid manipulators to allow the rotation of the grid by a value defined within the Step dialog box.
r
q
q
according to the user-defined viewpoint reflect lines do not move. but you can move the eye. or the grid manipulators to display a rotation direction and an axis. Press and hold the Shift key to rotate in the opposite direction. slide the pointer about the rotation axis. Click the dot and still holding the mousekey down.

You can therefore create several such analyses on different set of surfaces or on the same set of surfaces but using a different viewpoint. When you click the User-defined Eye icon . You can transfer a reflect line analysis from an element to another. A Reflect Lines Analysis is created in the specification tree. all the elements included in this geometrical set are automatically selected too. Reflect lines are displayed on that surface provided the grid orientation is adequate. meaning that you can move the geometry around while keeping the reflect lines static according to that viewpoint. The reflect lines will appear or disappear respectively.
. When you select the geometrical set as an input in the specification tree. and attenuation. Profiler & Optimizer
q
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You can select and deselect the analyzed surfaces. To do this. for example. auto detection. or using the Edit contextual menu to precisely define its location. they can be edited using the contextual menu in the specification tree. simply choose the Keep this reflection line or Keep all reflection lines from the contextual menu displayed when right-clicking either a reflection line itself or one of the grid neons. to remove it. a dot is displayed (you need to zoom out
q
q
to locate it) defining the eye and its position.
q
You can drop reflect lines onto the analyzed element. As reflect line analyses are objects as such. Select the surface on which the analysis existed. Click OK in the Reflection dialog box
r
r
Available capabilities from the dashboard are: datum creation. while applying the analysis. The reflect lines are frozen according to that direction. You can moved the eye using manipulators. To do this: r Double-click the reflect line analysis from the specification tree
r
q
q
Select the surface on which you wish to apply the analysis. A curve corresponding to the reflection line is created.FreeStyle Shaper.

Select the surface to be analyzed.
2. all points of the surface at which the curvature value is null. Drag and Drop the compass onto the zx plane. The system detects. Click the Inflection Line icon in the Shape Analysis toolbar. within the planes parallel to the one defined by the compass. 3. It contains a surface on which a cutting plane Analysis has been performed.FreeStyle Shaper. 1. Open the InflectionLine1. and links them together into curves. meaning that in these points.CATPart document. the curvature orientation is changing. Profiler & Optimizer
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Creating Inflection Lines
This task shows how to create inflection lines on a surface for analysis purposes. Inflection lines are curves which curvature value necessarily is 0.
.

inflection lines are automatically displayed on the surface.FreeStyle Shaper.
. Profiler & Optimizer
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The compass is automatically positioned on the selected element. 4. and the Inflection lines dialog box is displayed. Define the plane used to compute the inflection lines on the surface:
q
the compass base plane (Compass Plane) the surface parametric directions (Parametric)
q
Once the local plane is defined.

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5.
.FreeStyle Shaper.
for example. Click OK in the Inflection Line dialog box to create the analysis as an element in the specification tree. Grab the compass by its tip (w) and drag it along. to see the
The compass base plane's orientation being modified. the inflection lines are updated accordingly:
7. 6. Hide the Cutting Plane analysis. using the Hide/Show icon inflection lines better.

Used in conjunction with the Inflection area option of the Surfacic Curvature Analysis command.FreeStyle Shaper.
q
q
. you can notice that these lines always are created within the blue. Profiler & Optimizer
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q
Creating and retaining inflection lines on a surface is especially useful to determine at which points the curvature of the intersection between the cutting planes and the surface is null. When you select the geometrical set as an input in the specification tree. all the elements included in this geometrical set are automatically selected too.

The resulting roof surface will look like this:
. Profiler & Optimizer
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Interoperability Between the FreeStyle Shaper and Optimizer
The following scenario illustrates.FreeStyle Shaper. This scenario is performed in P2 mode. in an industrial environment. It consists in creating the surface corresponding to the roof of a car. how to work with the FreeStyle Shaper and Optimizer specific commands. because some of the capabilities used throughout the scenario are available with the P2 configuration only (all FreeStyle Optimizer capabilities for example)
Creating Four-Points Patches Deforming the Surface Limits Fitting the Surface to a Cloud of Points Analyzing the Surface Smoothing the Surface Extracting the Surface
This scenario is accomplished in ten minutes.

1.
3. It contains windshields of the car. You can hide the Reflect Line Analysis for the moment. style curves limiting these (windshield boundaries) style curves. Click the four style curve end-points (yellow styling D curves) as limits to the roof patch. Profiler & Optimizer
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Creating Four-Points Patches
This task explains how to create a pad from a sketch in the Part Design Workbench. Click the Four-Point Patch icon
.CATPart document. and curvature analyses applied onto each of these styling curves.FreeStyle Shaper. the end point are easily detected. onto which the roof should be mapped. Because the auto detection capability has been activated. Open the RoofStart.
. Check the Snap On Vertex
icon from the FreeStyle Dashboard to snap onto the
closest corner when moving the pointer close to the geometry
2.
The patch is created.

Choose the Top View icon from the View toolbar. Select the surface you just created and click the Control Points icon The Control Points dialog box is displayed. Hide the three Curvature Analyses. Profiler & Optimizer
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Deforming The Surface Limits
This task explains how to modify the surface limits within a given plane (in 2D) to get them to coincide with the already existing geometry. 2.
This will allow you to position the symmetry plane according to the current plane. 1. using the Show/Hide contextual menu from the specification tree. The RoofStart.CATPart document still is open from the previous task. normal to the ZX reference plane.FreeStyle Shaper.
. Drag the compass by its base and drop it to position it.
4. 3.
.

6. Choose the following deformation options from the dialog box:
q
Support: Translation along mesh lines
q
Law: Move selected points using a convex law
8.
A message is issued asking whether you want to use the current plane. Profiler & Optimizer
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5.FreeStyle Shaper. Click the top front control point. 9. as the symmetry plane
. Click OK. Use the manipulators on one of the corner control points to bring it closer to the orange
. The whole front mesh line is selected.
7. that is the one you defined above. then press and hold the Shift key then click the bottom front control point. Click the Symmetry icon
from the Control Points dialog box.

From the Control Points dialog box.
10.
.
The mesh line takes the global shape of the reference curve. Repeat this operation with the rear mesh line and reference curve. select new options:
q
Support: Translation along local tangents Law: Move selected points identically
q
12. Repeat this step with the rear mesh line and reference curve. 11.FreeStyle Shaper. Profiler & Optimizer
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reference curve. Select the front mesh line and drag it towards the reference curve so that it is superimposed. even though it does not match it perfectly yet.

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13.
.
You need to iterate on the front and rear mesh lines. Select one of the side mesh lines and bring it closer to the orange reference curve till the patch corner reaches the curve's end points. using the same options to reach a satisfying level of superimposition.

14. Select each patch corner point and move it exactly onto the reference corner point. You need to move them along the Y direction only.FreeStyle Shaper. to move them closer to the patch center. 16. Move the inner control points 2 by 2. You need to move them along both X and Y.
The patch now has the shape given by the reference curves.
. Move each side control points to superimpose the patch boundaries and reference curves. Profiler & Optimizer
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For further tuning you need to zoom in and move single control points. 15. using the Shift key.

Reset the compass to the default position using the 2. is active in
. Profiler & Optimizer
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Fitting The Surface To a Cloud of Points
This task explains how to fit the deformed surface to an existing cloud of points.
and
icons. Select the roof patch as the source element.FreeStyle Shaper.
3.
The Fit To Geometry dialog box is displayed and texts indicating the fitting constraints are displayed on the surface boundaries provided the Continuity icon the Dashboard.
1. The RoofStart. Click the Fit to Geometry icon
.CATPart document still is open from the previous task.

It may be easier to select it from the specification tree than from the geometry itself. Click Fit in the dialog box.3 make sure the Impose direction option is unchecked
r
r
and from the Dashboard. V Orders icon Nu=4 and Nv=4
and make sure they are
5. click the U. Select the Cloud of points as the target element.FreeStyle Shaper. Profiler & Optimizer
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4.
.5 and smoothing to 0. Set the following parameters in the dialog box:
r
set the fitting tension to 0. Click OK in the dialog box.
7. 6.

Set the following parameters in the dialog box:
q
Check the Normal distance direction Check the Limited Color Range mode
q
4. 3.FreeStyle Shaper.
The Distance dialog box is displayed. 1. Select the fitted surface as the first element. a reflect line analysis
The RoofStart.
2. a distance analysis 2. Click the Distance Analysis icon .CATPart document still is open from the previous task. Profiler & Optimizer
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Analyzing The Surface
This task explains how to analyze the surface. Click the More button to display further options:
q
Check the Color scale button to display the color range Check the Min/Max values to display these values on the geometry
q
. once it has been fitted onto the cloud of points. This is done via two different analyses: 1.

15mm below the surface
r
5.15mm above the surface
r
green for all points between 0.
Points are dynamically displayed and the minimum and maximum deviations are identified on the surface.15 and -0. set the colors to: r blue for all points located over 0. Check the Second set button then select the cloud of points.15mm away from the surface red for all points located beyond -0. Profiler & Optimizer
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q
From the displayed color range.
.FreeStyle Shaper.

1. then select the roof patch to apply the reflect line analysis. and red for parts lying below the cloud. Click the front and rear windshields to remove the current reflect lines.
9.
The parts of the surface that lie above the cloud are identified by blue dots. Click OK. This means that the surface needs to be smoothed further.
. From the specification tree. 8. Choose the Top View icon from the View toolbar.
The Reflection Lines dialog box is displayed and a grid of neons appears in the geometry.
7. double-click the Reflect Line Analysis.
10. so that all points turn green indicating a perfect matching with the cloud of points. Profiler & Optimizer
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6.FreeStyle Shaper. From the specification tree. choose the Show/Hide contextual menu on the distance analysis to hide it for the moment.

The Tuner dialog box is displayed. 14. Set the neons parameters to N=21 (number of neons in grid) and D=150 (distance between two neons). 3000 and click OK.
This moves the eye directly above the roof patch. Zoom out till you locate the green dot symbolizing the analysis eye. Profiler & Optimizer
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11.FreeStyle Shaper. then OK in the Reflection Lines dialog box. 12. Right-click on this eye and choose the Edit contextual menu. 0.
The analysis is visible on the roof patch:
. Click Close in the Tuner dialog box. 13.
15. Key in the eye's coordinates: 1850.

Choose the Tools -> Options menu item. The RoofStart.
The Control Points dialog box is displayed. 6. to increase the number of mesh lines in U and V respectively. set the attenuation value to 0.CATPart document still is open from the previous task.
4. Shape -> FreeStyle tab. Select the roof surface and click the Control Points icon .FreeStyle Shaper. Profiler & Optimizer
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Smoothing The Surface
This task explains how to further smooth the surface onto the cloud of points following the distance and reflect line analyses. Select the central U mesh line.
1. Drag the compass by its base and drop it to position it. and you need to display the distance analysis again.
Set the order numbers to Nu=5 and Nv=7 using the contextual menu. 2.01 and click OK. using the Show/Hide contextual menu. V Orders icon
. normal to the ZX reference plane. From the Dashboard. This to set it within the symmetry plane. 3. Choose the following options:
q
Support: Translation along local normals Law: Move points identically Symmetry: use the current plane
q
q
5.
. This brings more flexibility in terms of modifications. click the U.

that is lying between -0. You may also need to decrease the step and attenuation values and the number in U and V to reach a smoothed surface. 8.
.15mm and 0. Press and hold the Shift key. displaying mostly green dots. Profiler & Optimizer
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7. then decrease the deformation step to 0. and click the arrow up or down till you display green points all over the surface. i. You can also choose the Freeze contextual menu.15 mm from the cloud of points.e. Right-click the arrow to display the contextual menu and choose Edit.FreeStyle Shaper.75. to avoid selecting points from the cloud.
9.

and click to define a corner of the new surface. Profiler & Optimizer
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Extracting The Final Surface
This task explains how to extract a shorter surface from the smoothed surface in order to remove the rugged ends of the surface. Select the roof surface.
3.FreeStyle Shaper. The RoofStart. Drag the pointer over the side of the surface to the green area limit and click to define the second corner definition.
2. Click the Geometry Extraction icon . towards the rear of the surface.CATPart document still is open from the previous task. move the pointer to the limit of the green area.
. 1.

FreeStyle Shaper. You can also modify the final surface color using the Properties contextual menu. Hide the initial surface using the Hide/Show contextual menu. Double-click the Reflect Line Analysis from the specification tree. 5.
. Profiler & Optimizer
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The new surface is created. and transfer it by successively clicking the initial surface then the new one.
4. Graphic tab.
The final roof surface looks like this:
.

select the profile. It is used on the same type of elements yet taking the design capabilities one step further. Profiler & Optimizer
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Using the FreeStyle Profiler
The FreeStyle Profiler offers complementary capabilities to the FreeStyle Shaper.
.FreeStyle Shaper. display and manipulate the parameters. spine. guide and reference profiles if needed.
Create a net surface : select the guide and profile curves. choose the dominant curves Create a styling sweep: choose the sweep type.

The dialog box is updated with the number of guides and profiles selected. Profiler & Optimizer
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Creating a Net Surface
This command is only available with the FreeStyle Profiler.
3. The guides (0) text is highlighted. based on an existing set of curves (the net).
The Net Surface dialog box is displayed.FreeStyle Shaper.
. This task explains how to create a surface. one after the other.CATPart document.
2. Click the Net Surface icon . 1. Open the NetSurface1. Click the profiles text in the dialog box and select all the profile curves in the geometry. Successively select one or more guide curves in the geometry (using the Ctlr key for multiselection).

FreeStyle Shaper.
The selected curve must be isoparametric. Click the Display>> text to display the maximum information. guide or profile.
The information option enables you to display or not the tags. This means that the surface segmentation is based on these specific curves segmentation. Click the Copy (d) mesh on surface (it highlights) to copy the geometry of the dominant guide curve and the dominant profile onto the net surface.
Without option highlighted
With option highlighted
6. If you click on a curve text.
. the curve then becomes the dominant curve.
4. Click the <<Settings text to access advanced settings. Profiler & Optimizer
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You noticed that the first guide and profile you selected is identified by a (d) standing for "dominant".
5.

Four types of moving frames are available:
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q
Perpendicular to the dominant guiding curve
q
PseudoPerpendicular to the dominant guiding curve
. press and hold Shift while clicking to move back. Activate the moving frame. you can click the moving frame to change its type.FreeStyle Shaper. or right-click to display the contextual menu. In the geometry. The moving frame is used to define how the profile's position along the guiding curve. Profiler & Optimizer
7.

Click Apply to create the surface.
. If you are not satisfied with the results.FreeStyle Shaper. you can click another guide or curve to modify the surface. Profiler & Optimizer
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q
Two guiding curves and perpendicular to the dominant guiding curve
q
Two guiding curves and pseudoperpendicular to the dominant guiding curve
q
Parallel to plane
8.

appears. and furtive display. In case the selected guide or profile lies on more than one support.
.
You can create a net surface by selecting two or more profiles and no guide or two or more guides and no profile.FreeStyle Shaper. Available capabilities from the dashboard are: datum creation. continuities. the Please refer to Selecting a Support for further information. temporary analysis. Click OK to confirm the net surface creation. Profiler & Optimizer
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9.

This task explains how to create a swept surface. Click the Sweep icon .
Example of Simple Sweep
Resulting Sweep
.
2. Open the StylingSweep1. Profiler & Optimizer
Creating a Styling Sweep
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This command is only available with the FreeStyle Profiler.FreeStyle Shaper.
The Styling Sweep dialog box is displayed.CATPart document. Choose the sweep type by clicking on the icons on the left. 1. Simple: creates a surface based on two curves (profile and spine).
Four types are available:
1. based on a profile swept along a spine.

Profiler & Optimizer
2. Sweep & fit: creates a surface based on three curves (profile.FreeStyle Shaper. There is no relimitation of the swept surface onto the guiding curve. spine and guide). spine and guide). then the calculation of the sweep stops. If the profile is extrapolated half its length. The swept surface is relimited onto the guiding curve. There is no deformation of the swept profile according to the guiding curve. The swept profile is deformed onto the guiding curve. 3. and is no longer in contact with the guide.
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. Sweep & snap: creates a surface based on three curves (profile.

.FreeStyle Shaper. spine. and information. and one or more reference profiles). the corresponding parameter is visible in the 3D geometry. moving frame.
q
Click the values in the dialog box to edit them.
Be careful not to over-constrain the surface by setting low values for both deviation and V order. Click the <<Settings text in the dialog box to view and select the settings:
You can define the following parameters that will affect the quality of the resulting swept surface:
q
the maximum V order allowed for the resulting swept surface.
3. This would result in an increase of segments for the generated swept surface. tangency conditions are taken into account at the contact points between the reference profile(s) and spine and guiding curve. Click Selection>> then Display in the dialog box to view and select the display parameters: limits points. in order to decrease the number of control points and segments on the resulting swept surface. Moreover. ranging between two and sixteen. 4. guide. The swept profile is deformed onto the guiding curve. the U order being defined by the profile curve's order. Sweep near profiles: creates a surface based on at least four curves (profile.
When the texts are displayed in white. Profiler & Optimizer
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4. the maximum deviation between the exact surface and the resulting surface. This value is the maximum allowed. but not necessarily the resulting surface's order if the system finds a better solution.

Profiler & Optimizer
5. In the moving frame representation:
q
T is the tangent to the spine at the current point B is the vectorial product between T and the compass direction N is the vectorial product between T and B. while constantly remaining tangent to the spine. Activate the moving frame. Four types of moving frames are available:
1. In the geometry. On contour: the profile translation is recomputed at every point of the spine. press and hold Shift while clicking to move back.FreeStyle Shaper.
The current type is displayed when passing the pointer over the moving frame.
4.
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The moving frame is used to define how the profile is swept along the spine. meaning the profile follows the spine contour. Fixed direction: the profile is translated according to the compass orientation. Translation: the profile is translated along the spine
2.
q
q
In the last two cases. or use the quick compass orientation capability. to set the direction according to the compass orientation definition. Tangent to contour: the profile translated according to the compass orientation. You can move the frame along the spine using the manipulator at the moving frame's origin. you can click the moving frame to change its type.
.
q
the compass should not be tangent to the curve. The spine should not have inflexion points. or rightclick to display the contextual menu. q you need to drag and drop the compass onto the geometry.
3. The moving frame is not available with the sweep near profile.

appears. attenuation. 7. Profiler & Optimizer
6. depending on the chosen sweep type. The Information option displays the role of the selected elements in the geometry: profile. provided the Continuity icon is active from the dashboard.
Note that all continuities are not always available. and the geometry itself. spine. Capabilities are available from the contextual menu when right-clicking a limit point.
Available capabilities from the dashboard are: datum creation.
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They allow you to redefine the surface limits on the spine/guide. and furtive display. In that case. or curvature continuity) using the contextual menu on the displayed information. the Please refer to Selecting a Support for further information. when selected. Click OK to create the styling sweep. Activate the limit points. you can set the type of continuity to be taken into account (point.FreeStyle Shaper. you can use the Contact Points icon manipulator on the surface and modify its limits. Styling sweeps cannot be created using canonical profiles. and guide. temporary analysis.
to display the
In case the selected guide or profile lies on more than one support. auto detection. continuity. contact points.
q
You can select surface edges as the spine and guide.
. These points show up only when the surface extends beyond the reference profile. tangency.
q
Similarly. and are limited by the spine or guide's length.

or Remove Geometrical Set or Change Geometrical Set contextual menus. Manage ordered geometrical sets: select an Ordered Geometrical Set in the specification tree. Profiler & Optimizer
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Managing Geometrical Sets and Ordered Geometrical Sets
Insert geometrical sets: select the branch where the new geometrical set should be inserted and choose the Insert -> Geometrical Set menu command. use the Insert -> Ordered Geometrical Set menu command.FreeStyle Shaper. Hide/show geometrical sets or ordered geometrical sets and their contents: select the geometrical set or the geometrical set to be hidden and use the Hide/Show capabilities.
. Manage geometrical sets: select a Geometrical Set in the specification tree. use the Insert > Geometrical Set menu command.

1.
2. If all selected entities belong to the same geometrical set. the father of the new geometrical set is automatically set to the father of these entities. The Features list displays the elements to be contained in the new geometrical set. Open the ConnectChecker2. using the Define in Work Object contextual command. This element defines the father location for the insertion of the new geometrical set.
3. or any . Profiler & Optimizer
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Inserting Geometrical Sets
This task shows how to insert a new geometrical set entity in the specification tree.CATPart document already containing at least one geometrical set and geometric elements. In the specification tree. Select the Insert -> Geometrical Set menu command. select the element at which level you want the new geometrical set to be inserted.
4.CATPart document.
The Insert Geometrical Set dialog box is displayed.
. Enter the name of the new geometrical set. Select additional entities that are to be included in the new geometrical set.FreeStyle Shaper.

CATIA displays this new Geometrical_Set..
The result is immediate. Select the Geometrical_Set.x.1 and is still active.1 in the specification tree. 7. in the specification tree.
The selected geometrical set has been moved last in the initial Geometrical_Set. It is created after the last current geometrical set and is underlined.
6.object -> Change Geometrical Set.
. incrementing its name in relation to the pre-existing bodies. Click OK to create the geometrical set at the desired location. indicating that it is the active geometrical set.FreeStyle Shaper. then click OK in the Change Body dialog box.. contextual command on the newly created geometrical set. Profiler & Optimizer
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5. Use the Geometrical_Set2.

These management functions have no impact on the part geometry. such as Generative Structural Analysis for example. a Geometrical Set automatically becomes the current body.FreeStyle Shaper. i. Profiler & Optimizer
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Managing Geometrical Sets
Geometrical sets enable to gather various features in a same set or sub-set and organize the specification tree when it becomes too complex or too long.
q
You can insert and manipulate geometrical sets in the specification tree in much the same way as you manage files in folders. You can put any element you wish in the geometrical set. This involves:
q
inserting a geometrical set removing a geometrical set changing body sorting the contents of a geometrical set reordering components
q
q
q
q
You will find other useful information in the Managing Groups and Hiding/Showing chapters. 2. menu item The External View dialog box is displayed. is visible and not any intermediate state of the Hybrid Body. the result of all the operations performed on geometry. This also means that only the results of the Hybrid Body.e. 3. Select the element belonging to a Geometrical Set that should always been seen as the current element when working with an external application. You can define the Generative Shape Design feature that is to be seen when working with another application... You should refer to the Copying and Pasting section for information about how geometrical sets can be used in a part edition context. The order of these elements is not meaningful as their access as well as their visualization is managed independently and without any rule. To do this. it does not have to be structured in a logical way. Click OK in the dialog box.
q
q
q
q
. while in the Generative Shape Design workbench: 1. When loading the Generative Shape Design workbench. Choose the Tools -> External View. This task shows how to manage geometrical sets within the specification tree.

. 4. Note that you cannot deselect an external view element and that only one element can be selected at the same time. You can also open the GeometricalSets2. Select the Insert -> Geometrical Set menu command.
Inserting a Geometrical Set
1. Open any . Select additional entities that are to be included in the new geometrical set.CATPart document. All destinations present in the document are listed allowing you to select one to be the father without scanning the specification tree. The dialog box will display the name of the currently selected element. even if other elements are created later in the . The Features list displays the elements to be contained in the new geometrical set. 3. choose the Tools -> External View.
.FreeStyle Shaper. menu item again. They can be: r geometrical sets
r
parts
5. Use the Father drop-down list to choose the body where the new geometrical set is to be inserted. select an element as the location of the new geometrical set. This element will be considered as a child of the new geometrical set and can be a geometrical set or a feature. This also allows you to change elements through the selection of another element. chronologically speaking. In the specification tree.CATPart document containing Geometrical Sets. Profiler & Optimizer
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The selected element will be the visible element in other applications. The Insert Geometrical Set dialog box is displayed. To check whether an external view element has already been specified.
2.CATPart document.. Enter the name of the new geometrical set.

FreeStyle Shaper.
q
You cannot create a geometrical set within an ordered geometrical set and vice versa.
The result is immediate.
. Right-click the geometrical set then select the Delete contextual command. indicating that it is the active geometrical set.
Removing a Geometrical Set
Two methods are available: q If you want to delete the geometrical set and all its contents: 1.
q
If you want to delete the geometrical set but keep its contents: This is only possible when the father location of the geometrical set is another geometrical set.
q
You can check the Create a Geometrical Set when creating a new part option in Tools -> Options -> Infrastructure -> Part Infrastructure -> Part Document tab if you wish to create a geometrical set as soon as you create a new part. Profiler & Optimizer
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If all selected entities belong to the same geometrical set. in the specification tree. The next created element is created within this geometrical set. the father of the new geometrical set is automatically set to the father of these entities. This Insert Geometrical Set dialog box is only available with the Generative Shape Design 2 product. CATIA displays this new Geometrical Set. please refer to the Customizing section of the Part Design User's Guide. For more information about this option. It is created after the last current geometrical set and is underlined. This is not possible when the father location is a root geometrical set. Click OK to create the geometrical set at the desired location. incrementing its name in relation to the pre-existing bodies.x. 6.

object -> Change Geometrical Set. The geometrical set is removed and its constituent entities are included in the father geometrical set. the contextual menu is not available. Profiler & Optimizer
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1.
Multi-selection of elements of different types is supported. From the specification tree. item from the contextual menu.FreeStyle Shaper. However.
Moving a Geometrical Set to a New Body
1. The list of destinations is alphabetically sorted.
The Change Body dialog box is displayed. note that in this case. Right-click the desired geometrical set then select the Geometrical Set. select the element then choose the Geometrical Set.. and that you can access this capability using the Edit menu item. Indeed this geometrical set is considered as private and can only be deleted globally.x object -> Remove Geometrical Set contextual command.
You cannot delete a feature within a geometrical set created on the fly..
.

or using the drop-down list from the dialog box.FreeStyle Shaper. By default. before which the moved geometrical set will be located. Click OK to move the geometrical set to the new body.
The element selected first is moved to its new location in the specification tree. the geometrical set is positioned last within the new body. you can select any element in the new body. Profiler & Optimizer
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2. Select the element above which the one you already selected is to be inserted. if you select a body.
You can do so by selecting the Body in the specification tree.
3. In this case the Destination field of the Change Body dialog box is automatically updated with the Body to which this second element belongs.
You can directly select this positioning element. but geometry remains unchanged. However.3. Here we selected Geometrical_Set. Select the Destination body where the geometrical set is to be located.
.
4.

all the parent elements are highlighted prior to the move. In this case. at a time. Profiler & Optimizer
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q
Check the Change body unshared parents option to move all parents of the first selected element to its new location. i.1.
. regardless of whether these parents are used (shared) by any other element of the initial body.
q
You can move a whole branch.FreeStyle Shaper. provided these parents are not shared by any other element of the initial body. In this case.e.3 last in Geometrical_Set. all the unshared parents are highlighted prior to the move.
q
Check the Change body all parents option to move all parents of the first selected element to its new location. Here we moved Geometrical_Set. a whole body and its contents.

The geometry remains unchanged. use the Auto-sort capability to reorder the Geometrical Set contents in the specification tree (geometry itself is not affected).1 object -> AutoSort command. when the geometric elements no longer appear in the logical creation order. Profiler & Optimizer
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Sorting the Contents of a Geometrical Set
You may need to sort the contents of a Geometrical Set. In that case.
Instantly. Right-click the Geometrical_Set.
.1 from the specification and choose the Geometrical_Set.1 contains two extruded surfaces based on point-point lines. The Geometrical_Set.FreeStyle Shaper. The specification tree looks like this:
1. the contents of the Geometrical Set are reorganized to show the logical creation process.

It allows you to make the Replace option possible only for features located below the feature in Work Object and in the same branch. The Reorder Children dialog box is displayed. the Do replace only for elements situated after the In Work Object option is available in Tools -> Options -> Part Infrastructure -> General tab.FreeStyle Shaper. Use the arrows to move an element up or down. 3. Select an element.1 from the specification tree and choose the Ordered Geometrical Set. 1. Right-click the Geometrical_Set. To manage this capability. 2.1 object > Reorder Children command. Please refer to the Replacing or Moving Elements chapter in the Part Design User's Guide. Profiler & Optimizer
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Reordering Components within a Geometrical Set
This capability enables you to reorder elements inside the same geometrical set.
Reordering Features
The Reorder command allows you to move a feature in a Geometrical Set. These features can be: q solids
q
shape features sketches
q
Replacing Features
This capability is only available on shape features.
.

even if other elements are created later in the . The External View dialog box is displayed. In an ordered geometrical set. such as Generative Structural Analysis for example. In the specification tree. This also allows you to change elements through the selection of another element. Profiler & Optimizer
Managing Ordered Geometrical Sets
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Geometrical sets enable to gather various features in a same set or sub-set. Click OK in the dialog box.. 3. 2.CATPart document containing Geometrical Sets. To do this. and absorption. This task shows how to manage ordered geometrical sets within the specification tree.. Creation features create a new object and modification features create a new state in an existing object as well as absorb the preceding state(s). choose the Tools -> External View. You can define the Generative Shape Design feature that is to be seen when working with another application. Absorbed features are no longer visible nor accessible..CATPart document. Choose the Tools -> External View. Open any . chronologically speaking. as if ''masked'' by their absorbing feature. Select the element belonging to a Geometrical Set that should always been seen as the current element when working with an external application. The selected element will be the visible element in other applications. select an element as the location of the new ordered geometrical set.
. The dialog box will display the name of the currently selected element. That is why ordered geometrical sets introduced notions of succession of steps that define the design. features in an ordered geometrical set can be set as current: a given step of the design creation is chosen and what is located after it is not accessible nor visible. this structure does not fit the design process. This element will be considered as a child of the new ordered geometrical set. menu item.FreeStyle Shaper. and Copying and Pasting chapters. Hiding/Showing. The order of these features is not meaningful as their access as well as their visualization is managed independently and without any rule.
Inserting an Ordered Geometrical Set
1.CATPart document.. However flexible. To check whether an external view element has already been specified. Unlike features within a geometrical set. while in the Generative Shape Design workbench: 1. Note that you cannot deselect an external view element and that only one element can be selected at the same time. Inserting an Ordered Geometrical Set does not break the succession of steps as the order applies to all the elements of a same root ordered geometrical set. This involves:
q
inserting an ordered geometrical set defining an in work object visualizing features within an ordered geometrical set removing an ordered geometrical set removing a feature within an ordered geometrical set sorting the contents of an ordered geometrical set reordering components within an ordered geometrical set reordering features modifying children replacing features inserting and deleting inside and ordered geometrical set
q
q
q
q
q
q
q
q
q
q
You will find other useful information in the Managing Groups. the order of apparition of features in the specification tree is consistent with the steps of creation of the design. menu item again. You can also open the OrderedGeometricalSets1.

x.
Visualizing features in an Ordered Geometrical Set
It can be useful to temporarily see its future geometry.
Defining an In Work Object
The next created element is created after the In Work object. Click OK to create the ordered geometrical set at the desired location. This Insert ordered geometrical set dialog box is only available with the Generative Shape Design 2 product. Profiler & Optimizer
2. For further information. refer to the Inserting a Body into an Ordered Geometrical Set chapter. They can be: r ordered geometrical sets
r
parts
By default the destination is the father of the current object. you can check the Future geometry option in Tools -> Options -> Part Infrastructure -> Display tab. in the specification tree.
The result is immediate.FreeStyle Shaper. 6.
. Enter the name of the new ordered geometrical set you wish to insert. Select the Insert -> Ordered Geometrical Set menu command. If all selected entities belong to the same ordered geometrical set. It allows you to also display the geometry located after the current feature.
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4. CATIA displays this new Ordered Geometrical Set. incrementing its name in relation to the pre-existing bodies. The Features list displays the elements to be contained in the new ordered geometrical set. Use the Father drop-down list to choose the body where the new ordered geometrical set is to be inserted. 3. If the new feature to be inserted is a modification feature. It is created after the last current ordered geometrical set and is underlined. indicating that it is the active ordered geometrical set. The Insert ordered geometrical set dialog box is displayed. By default the ordered geometrical set is created after the current feature. Select additional entities that are to be included in the new ordered geometrical set. All destinations present in the document are listed allowing you to select one to be the father without scanning the specification tree.
q
You can insert an ordered geometrical set after the current feature.
q
You can now insert a body into an ordered geometrical set. To do so. You cannot create an ordered geometrical set within a geometrical set and vice versa. 5. the father of the new ordered geometrical set is automatically set to the father of these entities. q Only features that come before the current object and that are not absorbed by any feature preceding the current object are visualized in the specification tree. features after the In Work object may be rerouted to the new created feature.

the selection of Offset. changing the color of a modification feature modifies the color of the initial state.1 is absorbed by Split. when editing Extrude. Profiler & Optimizer
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A color assigned to a feature is propagated to all the features that successively modify this feature and so on. To ensure the consistency between the visualization in the 3D geometry and the selection in the specification tree. if you want to allow the selection of geometrical elements absorbed by other elements or the selection of geometrical elements located after the element being created.
Selecting Features within an Ordered Geometrical Set
The selection of features located after the current feature or absorbed features is not possible. We advise you not to check these options but rather work in a geometrical set environment. If these options are unchecked. This is why it is possible to set a specific color only on creation features. Therefore. features that cannot be visualized in the 3D geometry cannot either be selected in the specification tree. As a consequence.
However. Here.
The same behavior applies on Show/No show attributes. for instance.1 is not possible because Offset. the application displays a tooltip explaining why it is not possible.1. you can check the Enable selection of drawn geometry or Enable the selection of future geometry options in Tools -> Options -> Part Infrastructure -> General tab. Therefore the color of Extrude.1. A black sign indicates that this selection is not possible.FreeStyle Shaper.1 is located after Extrude. the succession of steps of the ordered geometrical set is no longer respected.1.1 which is the current object. selecting elements whose geometry is not visible any more is not possible.
Here Extrude.
.1 is propagated onto Split. Additionally.

Therefore the deleted feature will be replaced by the modified feature of upper level. In our scenario.1 contains a line based on two points lines.
Sorting the Contents of an Ordered Geometrical Set
You may need to sort the contents of an ordered geometrical set. The geometry remains unchanged.FreeStyle Shaper. use the Auto-sort capability to reorder the ordered geometrical set contents in the specification tree.
Removing a Feature within an Ordered Geometrical Set
1. Offset.
Instantly. It may be the case if you enabled the selection of drawn or future geometry options. Right-click the Geometrical_Set. Split. The ordered geometrical set and all its contents are deleted.
q
deletion of a creation feature: no reroute is possible.
q
deletion of a modification feature: the system reroutes the children on the element that is modified. As a consequence. The specification tree looks like this:
1.1 from the specification and choose the Ordered Geometrical Set. Datum features are put first in the specification tree. Right-click the feature then select the Delete contextual command. In that case.1.1 now points Extrude. Profiler & Optimizer
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Removing an Ordered Geometrical Set
1.1 is deleted.
. Right-click the ordered geometrical set then select the Delete contextual command.1 object -> AutoSort command. the contents of the Ordered Geometrical Set are reorganized to show the logical creation process. The Ordered Geometrical Set. when the geometric elements no longer appear in the logical creation order.

CATPart document. you can see that Offset.1 (in blue) that splits Fill.1 (creation feature) before Split. Profiler & Optimizer
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Reordering Components within an Ordered Geometrical Set
This capability enables you to reorder elements inside the same ordered geometrical set.
If you define Split.1 does not modify Fill.1.
1. Here we chose to reorder Offset.1 from the specification tree and choose the Ordered Geometrical Set.1 by a purple vertical plane.1. 2.1 (modification feature).1.1 is now based upon Fill. Select the element to be rerouted. The Ordered Geometrical Set contains Split. and Offset.1 as the In Work object.1 up.1 was not rerouted since Offset. Split.FreeStyle Shaper. 4.1 (in red) is an offset of Split. Click OK.1 is now located before Split.
. The Reorder Children dialog box is displayed. Right-click the Ordered Geometrical Set.1 in the specification tree. Offset. 3. Use the arrow to move Offset.
Reordering a creation feature based upon a modification feature
Open the Reorder1.1 object -> Reorder Children command.

1 (in blue).2 would still split Split.1 (delimited by Sketch. The Reorder Children dialog box is displayed.1 object -> Reorder Children command.
.1.FreeStyle Shaper.2 (in blue) that splits Split. Split. Use the arrow to move Split. Right-click the Ordered Geometrical Set.2 (modification feature) before Split.1 from the specification tree and choose the Ordered Geometrical Set. Click OK.2 is rerouted onto the input feature modified by Split. The Ordered Geometrical Set contains Split.1 in purple).1 which comes after in the specification tree. that is Fill.2 is now located before Split.1 (modification feature).CATPart document. 2. Profiler & Optimizer
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Reordering a modification feature based upon a modification feature
Open the Reorder2. Select the element to be rerouted. Split.1 itself splits Fill.1 in the specification tree. Otherwise Split. 4.2 up. Split.
1.1 by a vertical plane. 3. Here we chose to reorder Split.

the feature just before the original position of the reordered feature becomes the In Work object.2.2 was rerouted onto Fill.
You can use the Scan command after the Reorder operation to see what moved step by step. the feature located just before the new position of the reordered feature becomes the In Work object.
2. we chose Line.x object -> Modifying children. Select the elements you wish to place first and last. This command is only available on sub-ordered geometrical sets. These features can be: q Generative Shape Design features
q
sketches
For further information.
An error message is issued if you try to move an element towards a position that breaks the order rules. The Edit dialog box opens with the First Element and Last element fields automatically valuated with the first and last elements of the ordered geometrical set.1 as the last element.
And since Split. Note that the feature defined as the In Work object after the Reorder operation is not affected by this operation from an update point of view: q when reordering upward.2. In our scenario. please refer to the Reordering Features chapter in the Part Design User's Guide.FreeStyle Shaper. as well as destroy it.1.2 now modifies Fill.
Reordering Features
The Reorder command allows you to move a feature in an Ordered Geometrical Set.
.1 as the first element and Split.1. Profiler & Optimizer
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Indeed. 1. when you edit Split.
Modifying Children
The Modify Children command allows you to modify the contents of an ordered geometrical set by selecting its first and last component.1 was rerouted onto Split. Split. you can notice that the Split.
q
when reordering downward. Right-click the sub-ordered geometrical set from the specification tree and choose the Ordered Geometrical Set.

Profiler & Optimizer
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3.
.
Switching From Ordered Geometrical Set to Geometrical Set
While in an ordered geometrical set environment. The Ordered Geometrical Set. 1. elements are rerouted in the father ordered geometrical set. As a consequence.
Replacing Features
Please refer to the Replacing or Moving Elements chapter in the Part Design User's Guide. if you do not want to work in an ordered environment any more).1 becomes Geometrical Set. Elements before or after the first and last elements are rerouted in the father ordered geometrical set. The Do replace only for elements situated after the In Work Object option is available in Tools -> Options -> Part Infrastructure -> General tab. It restricts the Replace capability only on features located before the feature in Work Object and in the same branch.1 object -> Switch to geometrical set command. Right-click the Ordered Geometrical Set.
The Modify children command also allows you to remove the sub-ordered geometrical set. you may want to switch to a geometrical set environment (for instance. As a consequence. We advise you not to check this option but rather work in a geometrical set environment.1 from the specification tree and choose the Ordered Geometrical Set. The specification tree is modified consequently. Click OK.1.FreeStyle Shaper. the succession of steps of the ordered geometrical set is no longer respected. Features after the current object that were not visualized in the ordered geometrical set are put in no show in the geometrical set.

1) must be rerouted to the inserted feature (Split.1 in the specification tree. This new feature absorbs EdgeFillet. This replacement applies to all the features inside the root ordered geometrical set (Ordered Geometrical Set.1). the links to the absorbed feature (EdgeFillet.1. Colors may be modified. the Insert and Delete commands may have impacts that result in replace actions based on absorption rules.FreeStyle Shaper. the edge fillet (Edge Fillet.1) is the current object.1) located after the inserted feature and to all the features located inside other ordered geometrical sets roots (here.CATPart document. Ordered Geometrical Set.
A split feature (Split.2). Here.1) is inserted just after EdgeFillet.1 and therefore the latter is no more displayed and cannot be referenced by any feature located after the Split.
To ensure the ordering rule.
. Switching from geometrical set to ordered geometrical set is not possible. Profiler & Optimizer
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This command is only available on a root ordered geometrical set. Open the OrderedGeometricalSets2.
q
q
Inserting and Deleting Inside an Ordered Geometrical Set
Inside an ordered geometrical set.

the design may require to create several modification states of a same feature. a copy of the copy is created. The replace actions performed by the Delete command are generally the opposite of the replace actions performed by Insert command. This example shows how to allow multiple modifications of EdgeFillet. Surface. the affected features (that is Extrapol. considered as an "intermediate state of design". In the beginning of every sub-set where this state of design will be used. In this example.1 feature. if inserting a Trim feature. which can be a modification feature). As a consequence. Open the OrderedGeometricalSets4. Open the OrderedGeometricalSets3. The update following the insertion may also produce an error and in this case the design will have to be modified so that the inserted feature is compatible with the entire design. the external link will have to reference this copy or its publication. deleting Split.FreeStyle Shaper. all inputs will be replaced by this feature but if deleting it.
As a consequence of the replace action. the Trim feature will be replaced by its main input). a feature can be the input of several features (all creation features. representing the exported view. In some cases.2 is a copy of EdgeFillet. in this case a warning message is issued. had we selected the other side of Split.1 or to the copies of the copy (imported views) will affect only the design in Sub OGS. Profiler & Optimizer
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This replace action may not be applicable. representing the imported view.1) become "not updated". The external link has to reference Surface. according to the order in the specification tree. A copy of the feature.CATPart document.1 by EdgeFillet.1.1 feature) would not have been possible. Using this construction. Using our example.2 or its publication.
Multiple references
Inside a root ordered geometrical set.1 and Offset. it is necessary to create a copy (Copy/Paste As Result With Link) of the last current feature in a new ordered geometrical set. bear in mind that deleting a feature can lead to a configuration different from the one preceding the insertion of a feature (for instance. Based on this mechanism stand two methodologies for: q multiple references to an intermediate state of design inside an ordered geometrical set.
External Links
The replace actions due to design modifications (insertion and deletion) do not affect external links (that is the links between an external element from the . is inserted just after it. modifications applied to EdgeFillet.1 leads to the replacement of Split. the replacement of the edge to extrapolate (defined in Extrapol.1. To ensure that the links will always reference the last state of design.CATPart document.1. This copy can possibly be published. Using our example.CATPart document and a feature inside an ordered geometrical set).
q
external links to the "end design" specified inside an ordered geometrical set. except for the last feature.
. Nevertheless. To do so. it is necessary to create copies (Copy/Paste As Result With Link).1.

FreeStyle Shaper.1 and so is the external link. Profiler & Optimizer
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A split feature is inserted after EdgeFillet.1. As a consequence.
.2 is rerouted to Split. Surface.

Right-click to display the contextual menu and choose the Hide/show command.
Hiding/Showing a Geometrical Set or an Ordered Geometrical Set
This contextual menu allows you to hide/show a geometrical set or an ordered geometrical set whether current or not. Indeed you can: q hide/show a complete geometrical set or ordered geometrical set
q
hide/show contents of a geometrical set or an ordered geometrical set hide/show an element while in a command hide/show an element belonging to an ordered geometrical set
q
q
Open any . or becomes visible. The geometrical set or ordered geometrical set is hidden.CATPart document to have an example with Geometrical Sets and the OrderedGeometricalSets1. 1. In the specification tree. Profiler & Optimizer
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Hiding/Showing Geometrical Sets or Ordered Geometrical Sets and Their Contents
This task shows how to use the Hide/Show command on different level of geometrical sets and ordered geometrical sets and for different purposes.CATPart document to have an example with Ordered Geometrical Sets. if it was hidden.
. select the geometrical set or ordered geometrical set you wish to hide/show 2. You can also open the GeometricalSets1. if it was visible.FreeStyle Shaper.CATPart document containing Geometrical Sets or Ordered Geometrical Sets.
Visible geometrical set
Hidden geometrical set
Hiding or Showing a geometrical set or an ordered geometrical set as a whole can also be done using the Hide/Show icon.

This method enables to quickly show an element of a geometrical set or an ordered geometrical set . Right-click and choose Geometrical_Set.x object -> Hide components contextual command to hide visible elements. Profiler & Optimizer
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It is not possible to hide a sub-ordered geometrical set using the Hide/Show contextual command.
. rather than using the Hide/Show contextual command: indeed when a geometrical set or an ordered geometrical set is in show. its contents are as well.
Hiding/Showing Contents of a Geometrical Set or Ordered Geometrical Set
This contextual menu allows you to hide/show all features in a geometrical set or an ordered geometrical set (even sketches).
Visible contents
Hidden contents
It is advised to use this method to hide contents of a geometrical set or an ordered geometrical set.x object -> Show components contextual command to restore the view if the elements were hidden. select the geometrical set or the ordered geometrical set whose solid elements you want to hide/show.FreeStyle Shaper. while using a command. In the specification tree. whether current or not.
Hiding/Showing an element while in a command
This contextual menu allows you to hide/show an element of the current geometrical set or ordered geometrical set. However you can use the Hide components contextual command as explained hereafter. or Geometrical_Set. 1. 2.

and choose the Hide/Show contextual command. Click OK in the Line dialog box to create the line. The selected element is hidden without exiting the currently active command.FreeStyle Shaper. Repeat the operation on the element again to re-display it. Profiler & Optimizer
1.
Hiding/Showing an element belonging to an Ordered Geometrical Set
This contextual menu allows you to hide/show a modification feature. Click the Line icon points to create a line. 4. If a modification feature is put in no show.
3. all features absorbed by this feature are in no show too. and select two
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2.
. Right-click the element to be hidden from the specification tree or the geometry.

1 is absorbed by Extrude. Right-click the element (Split. and choose the Hide/Show contextual command.
Note that you can hide/show all elements of a document.1 is also put in no show.1. Profiler & Optimizer
1. All Lines. All Elements. All Sketches. All Curves.FreeStyle Shaper. simply use the Tools -> Show or Tools -> Hide menu and choose the adequate element type (All Points. All Except Selected Elements). To do this. according to their type. All Bodies. Extrude.
. All Geometrical Sets. All Selected Elements. All Surfaces. All Planes.
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As Split. All Axis Systems.1) to be hidden from the specification tree or the geometry.

based on a step-by-step scenario composed of several tasks illustrating how to work with both surface and body type elements. Creating a Sketch and a Pad Creating a Surface Splitting the Pad Modifying the Splitting Surface
This scenario is accomplished in ten minutes. that is elements created using the Part Design workbench. it is always useful to have integrated design tools at one's disposal.FreeStyle Shaper. However in an industrial environment. The resulting body will look like this:
. creating forms and modifying them. The integration between the FreeStyle Shaper workbench and the Part Design workbench is described in the chapter. Profiler & Optimizer
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Interoperability with the Part Design Workbench
You can work in the FreeStyle Shaper/FreeStyle Optimizer workbench only.

Open a new . Click the Circle icon
.
3.
. 1. A rubberbanding circle follows the pointer as you drag it. Select xy plane to define the sketch plane. Profiler & Optimizer
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Creating a Sketch and a Pad
This task explains how to create a pad from a sketch in the Part Design Workbench. 6. Drag the pointer to see the circle being created.FreeStyle Shaper. Click once you are satisfied with the size of the circle.
2.CATPart document (see Opening a new CATPart Document) and activate the Part Design Workbench. Click where you wish the center of the circle to appear. Click the Sketcher icon .
4.
5.

and click OK to create the pad.
A cylindrical pad has been created using the Part Design workshop. Key in 150 in the power input entry area.FreeStyle Shaper. Click the Exit Sketcher icon Pad icon .
. Profiler & Optimizer
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7.
8.
then the
A default cylindrical pad is previewed.

The corresponding surface has been created in a plane parallel to that defined by the 3D compass.
The FreeStyle Shaper workbench is displayed. Now.
2. Profiler & Optimizer
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Creating a Surface
This task will show you how to enter the FreeStyle Shaper workbench.
3. See Creating Planar Patches for further details on the 3D compass capabilities and on creating planar surfaces. select the Top View icon to see the cylinder from the top. 1. Click at the center of the cylinder (where you clicked to create the circle sketch) press the Ctrl-key and drag the pointer so as to cover the cylinder face by the outline. click again.FreeStyle Shaper.
. choose FreeStyle from the Start -> Shape menu.
4. Select the Planar patch icon
. When you have reached the adequate size. From the View toolbar.
5.

drag and drop the compass onto the surface and drag the surface halfway of the cylinder length pulling on the z axis. Click the Isometric view icon .
. Profiler & Optimizer
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6. Reset the compass by clicking the Quick Compass Orientation then the
In Model or On Perch icons in the Current plane orientation toolbar. 8.FreeStyle Shaper.
7. In P2 mode.

The Part Design workbench is displayed again.FreeStyle Shaper.
4. make sure that it points in the right direction.
3. Now.
2.
. Select the created surface as the splitting plane. 1. Profiler & Optimizer
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Splitting the Pad
This task will show you how to split the cylinder by the surface. An arrow appears indicating the portion of body that will be kept. The cylinder has been split by the surface. choose Part Design from the Start -> Mechanical Design menu. Click OK in the Split Definition dialog box. Select the cylinder and click the Split
icon.

4. Select the surface and click the Control points icon .
Control points and mesh lines are displayed along with the Control Points dialog box.FreeStyle Shaper. 1. refer to Editing Surfaces Using Control Points for further details on surface modification. If needed. choose the Stretch selected points . Move the pointer over an edge mesh line and pull down so as to manually deform the surface. depending on the mode you are working in.
. 5. From the dialog box.
2.
Note that the Translation in the plane icon is the current support. Profiler & Optimizer
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Modifying the Splitting Surface
This task will show you how to modify the splitting surface. 3. Return to the FreeStyle Shaper workbench. The cylinder is automatically updated. Set the current plane to Flip to VW or YZ using the Current Plane
Orientation or Quick Compass Orientation toolbar.

FreeStyle Shaper. However in an industrial environment. If you need to deactivate the history. The integration between the FreeStyle Shaper workbench and the Wireframe workbench is described in the chapter. Creating Points Creating Lines Creating Planes Creating Circles When using these commands.
. Profiler & Optimizer
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Interoperability with the Wireframe Workbench
You can work in the FreeStyle Shaper/FreeStyle Optimizer workbench only. elements are created with their history. refer to Creating Datums. creating forms and modifying them. based on four tasks illustrating how to create wireframe geometry using the Wireframe workbench. it is always useful to have integrated design tools at one's disposal.

2. Click the Point icon . Use the combo to choose the desired point type. the point's coordinates are defined according to current the axis system. the point's coordinates within the document's default axis-system. The axis system must be different from the absolute axis. or simply find out. select a reference point. If you create a point using the coordinates method and an axis system is already defined and set as current. note that the Coordinates in absolute axis-system check button is added to the dialog box. As a consequence.
. Y.
When creating a point within a user-defined axis-system. Z coordinates in the current axis-system. Optionally.
q
The corresponding point is displayed. the point's coordinates are not displayed in the specification tree. 1. allowing you to be define.
Coordinates
q
Enter the X.
The Point Definition dialog box appears. Profiler & Optimizer
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Creating Points
This task shows the various methods for creating points: q by coordinates
q
on a curve on a plane on a surface at a circle/sphere center tangent point on a curve between
q
q
q
q
q
Open the Points3D1.CATPart document.FreeStyle Shaper.

q
If this point is not on the curve.
q
Select an option point to determine whether the new point is to be created: r at a given distance along the curve from the reference point
r
a given ratio between the reference point and the curve's extremity.FreeStyle Shaper. Profiler & Optimizer
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On curve
q
Select a curve Optionally. select a reference point. it is projected onto the curve. the curve's extremity is used as reference. If no point is selected.
.

q
click the Repeat object after OK if you wish to create equidistant points on the curve.
q
click the Middle Point button to display the mid-point of the curve. You can also: q click the Nearest extremity button to display the point at the nearest extremity of the curve.
The corresponding point is displayed. as described in Creating Multiple Points in the Wireframe and Surface User's Guide. it can be: r a geodesic distance: the distance is measured along the curve
r
an Euclidean distance: the distance is measured in relation to the reference point (absolute value). and to create all instances in a new geometrical set by checking the
.FreeStyle Shaper.
Be careful that the arrow is orientated towards the inside of the curve (providing the curve is not closed) when using the Middle Point option. If the reference point is located at the curve's extremity. You will also be able to create planes normal to the curve at these points. even if a ratio value is defined. the created point is always located at the end point of the curve. by checking the Create normal planes also button.
q
use the Reverse Direction button to display: r the point on the other side of the reference point (if a point was selected originally)
r
the point from the other extremity (if no point was selected originally). If a distance is specified. using the currently created point as the reference. Profiler & Optimizer
q
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Enter the distance or ratio value.

the reference point is the projection of the model's origin If the curve is a closed curve. If the button is not checked the instances are created in the current geometrical set . and highlights it (you can then select another one if you wish) or the system prompts you to manually select a reference point.FreeStyle Shaper. by default. Profiler & Optimizer
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Create in a new geometrical set button. either the system detects a vertex on the curve that can be used as a reference point. the projection of the model's origin on the plane is taken as reference. or it creates an extremum point. If the curve is infinite and no reference point is explicitly given.
q
If no point is selected.
. Optionally.
On plane
q
Select a plane.
q
q
Extremum points created on a closed curve are now aggregated under their parent command and put in no show in the specification tree. select a point to define a reference for computing coordinates in the plane.

Click in the plane to display a point.
If no surface is selected. the reference direction (H and V vectors) is computed as follows: With N the normal to the selected plane (reference plane).
q
. the reference direction would then be projected on the plane. H results from the vectorial product of Z and N (H = Z^N). Would the plane move. select a surface on which the point is projected normally to the plane. V = N^X and H = V^N. Otherwise.FreeStyle Shaper. If the norm of H is strictly positive then V results from the vectorial product of N and H (V = N^H). the behavior is the same. during an update for example. Furthermore. Profiler & Optimizer
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Optionally.

Enter a distance along the reference direction to display a point. Y. the surface's middle point is taken as reference. Profiler & Optimizer
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On surface
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Select the surface where the point is to be created.
q
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Circle/Sphere center
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Select a circle.
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. or Select a sphere or a portion of sphere. You can also use the contextual menu to specify the X. select a reference point. By default. or ellipse.FreeStyle Shaper. Z components of the reference direction. circular arc.
q
Optionally. You can select an element to take its orientation as reference direction or a plane to take its normal as reference direction.

A point is displayed at each tangent.
The MultiResult Management dialog box is displayed because several points are generated.FreeStyle Shaper. Profiler & Optimizer
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A point is displayed at the center of the selected element. to which only the closest point is created.
.
q
For further information.
Tangent on curve
q
Select a planar curve and a direction line.
q
Click YES: you can then select a reference element. Click NO: all the points are created. refer to the Managing Multi-Result Operations chapter.

5).
q
Parameters can be edited in the 3D geometry. For more information.
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Use the Reverse direction button to measure the ratio from the second selected point.
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. the point is located on the virtual line beyond the selected points.
If the ratio value is greater than 1. Profiler & Optimizer
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Between
q
Select any two points. 3. Click OK to create the point. use the Isolate contextual menu.
Be careful that the arrow is orientated towards the inside of the curve (providing the curve is not closed) when using the Middle Point option.xxx) is added to the specification tree. that is the percentage of the distance from the first selected point. For more information. refer to the Isolating Features chapter. To do so. The point (identified as Point. refer to the Editing Parameters chapter. You can also click Middle Point button to create a point at the exact midpoint (ratio = 0.FreeStyle Shaper.
q
Enter the ratio. at which the new point is to be. You can isolate a point in order to cut the links it has with the geometry used to create it.

Use the drop-down list to choose the desired line type. Profiler & Optimizer
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Creating Lines
This task shows the various methods for creating lines:
q
point to point point and direction angle or normal to curve tangent to curve normal to surface bisecting
q
q
q
q
q
It also shows you how to create a line up to an element.
q
Select two points.
The Line Definition dialog box is displayed.Point
This command is only available with the Generative Shape Design 2 product. Open the Lines1. Click the Line icon .
2.CATPart document.
. 1.
Defining the line type
Point .
A line type will be proposed automatically in some cases depending on your first element selection.FreeStyle Shaper. define the length type and automatically reselect the second point.

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A line is displayed between the two points. Proposed Start and End points of the new line are shown.

q

If needed, select a support surface. In this case a geodesic line is created, i.e. going from one point to the other according to the shortest distance along the surface geometry (blue line in the illustration below). If no surface is selected, the line is created between the two points based on the shortest distance.

If you select two points on closed surface (a cylinder for example), the result may be unstable. Therefore, it is advised to split the surface and only keep the part on which the geodesic line will lie. The geodesic line is not available with the Wireframe and Surface workbench.

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Specify the Start and End points of the new line, that is the line endpoint location in relation to the points initially selected. These Start and End points are necessarily beyond the selected points, meaning the line cannot be shorter than the distance between the initial points. Check the Mirrored extent option to create a line symmetrically in relation to the selected Start and End points.

q

The projections of the 3D point(s) must already exist on the selected support.

Point - Direction
q

Select a reference Point and a Direction line. A vector parallel to the direction line is displayed at the reference point. Proposed Start and End points of the new line are shown.

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q

Specify the Start and End points of the new line. The corresponding line is displayed.

The projections of the 3D point(s) must already exist on the selected support.

Angle or Normal to curve
q

Select a reference Curve and a Support surface containing that curve.

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- If the selected curve is planar, then the Support is set to Default (Plane). - If an explicit Support has been defined, a contextual menu is available to clear the selection.

q

Select a Point on the curve. Enter an Angle value.

q

A line is displayed at the given angle with respect to the tangent to the reference curve at the selected point. These elements are displayed in the plane tangent to the surface at the selected point. You can click on the Normal to Curve button to specify an angle of 90 degrees. Proposed Start and End points of the line are shown.

q

Specify the Start and End points of the new line. The corresponding line is displayed.

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q

Click the Repeat object after OK if you wish to create more lines with the same definition as the currently created line. In this case, the Object Repetition dialog box is displayed, and you key in the number of instances to be created before pressing OK.

As many lines as indicated in the dialog box are created, each separated from the initial line by a multiple of the angle value. You can select the Geometry on Support check box if you want to create a geodesic line onto a support surface. The figure below illustrates this case.

Geometry on support option not checked Geometry on support option checked This line type enables to edit the line's parameters. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry.

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Tangent to curve
q

Select a reference Curve and a point or another Curve to define the tangency. r if a point is selected (monotangent mode): a vector tangent to the curve is displayed at the selected point.
r

If a second curve is selected (or a point in bi-tangent mode), you need to select a support plane. The line will be tangent to both curves.

- If the selected curve is a line, then the Support is set to Default (Plane). - If an explicit Support has been defined, a contextual menu is available to clear the selection. When several solutions are possible, you can choose one (displayed in red) directly in the geometry, or using the Next Solution button.

Line tangent to curve at a given point Line tangent to two curves q Specify Start and End points to define the new line. The corresponding line is displayed.

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Normal to surface
q

Select a reference Surface and a Point. A vector normal to the surface is displayed at the reference point. Proposed Start and End points of the new line are shown.

If the point does not lie on the support surface, the minimum distance between the point and the surface is computed, and the vector normal to the surface is displayed at the resulted reference point.

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q

Specify Start and End points to define the new line. The corresponding line is displayed.

Bisecting
q

Select two lines. Their bisecting line is the line splitting in two equals parts the angle between these two lines. Select a point as the starting point for the line. By default it is the intersection of the bisecting line and the first selected line.

q

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q

Select the support surface onto which the bisecting line is to be projected, if needed. Specify the line's length in relation to its starting point (Start and End values for each side of the line in relation to the default end points). The corresponding bisecting line, is displayed. You can choose between two solutions, using the Next Solution button, or directly clicking the numbered arrows in the geometry.

q

q

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3. Click OK to create the line. The line (identified as Line.xxx) is added to the specification tree.

q

Regardless of the line type, Start and End values are specified by entering distance values or by using the graphic manipulators. Start and End values should not be the same. Check the Mirrored extent option to create a line symmetrically in relation to the selected Start point. It is only available with the Length Length type. In most cases, you can select a support on which the line is to be created. In this case, the selected point(s) is projected onto this support. You can reverse the direction of the line by either clicking the displayed vector or selecting the Reverse Direction button (not available with the point-point line type).

q

q

q

q

Creating a line up to an element
This capability allows you to create a line up to a point, a curve, or a surface.
q

It is available with all line types, but the Tangent to curve type.

Up to a point
q

Select a point in the Up-to 1 and/or Up-to 2 fields. Here is an example with the Bisecting line type, the Length Length type, and a point as Up-to 2 element.

the Length Length type. Here is an example with the PointPoint line type. the Up-to 1 field is grayed out with the Infinite Start Length type. The Up-to 1 field is grayed out if the Mirrored extent option is checked. It is only possible if the element is linear and lies on the same plane as the line being created. Profiler & Optimizer
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Up to a curve
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Select a curve in the Up-to 1 and/or Up-to 2 fields. The Up-to 1 and Up-to 2 fields are grayed out with the Infinite Length type. no extrapolation is performed if the Up-to element is a curve or a surface. However. and the surface as the Up-to 2 element. the Infinite End Length type.FreeStyle Shaper. then an extrapolation is performed. and a curve as the Up-to 1 element.
q
q
q
Defining the length type
. Here is an example with the PointDirection line type. In the case of the Point-Point line type.
q
If the selected Up-to element does not intersect with the line being created.
Up to a surface
q
Select a surface in the Up-to 1 and/or Up-to 2 fields. Start and End values cannot be negative. the Up-to 2 field is grayed out with the Infinite End Length type.

4. the Length type is selected. 3. Profiler & Optimizer
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Select the Length Type: r Length: the line will be defined according to the Start and End points values
r
Infinite: the line will be infinite Infinite Start Point: the line will be infinite from the Start point Infinite End Point: the line will be infinite from the End point
r
r
By default. 2.FreeStyle Shaper. Create the first point.
The Line dialog box is displayed. Double-click the Line icon . Check it to be able to later reuse the second point. The Start and/or the End points values will be greyed out when one of the Infinite options is chosen.
Reselecting automatically a second point
This capability is only available with the Point-Point line method. Create the second point.
. Click OK to create the first line.
The Reselect Second Point at next start option appears in the Line dialog box. 5. 1.

FreeStyle Shaper. For more information.
q
Parameters can be edited in the 3D geometry. Profiler & Optimizer
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The Line dialog box opens again with the first point initialized with the second point of the first line. For more information. simply uncheck the option or click Cancel in the Line dialog box. You can isolate a line in order to cut the links it has with the geometry used to create it. refer to the Editing Parameters chapter.
To stop the repeat action. To do so. use the Isolate contextual menu. Click OK to create the second line. refer to the Isolating Features chapter. 6.
q
.

Offset from plane
q
Select a reference Plane then enter an Offset value. which you can move using the graphic manipulator.
. Use the combo to choose the desired Plane type. 1.
The Plane Definition dialog box appears.FreeStyle Shaper.
Once you have defined the plane. Click the Plane icon . 2.CATPart document. Profiler & Optimizer
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Creating Planes
This task shows the various methods for creating planes:
q
q
offset from a plane parallel through point angle/normal to a plane through three points through two lines through a point and a line
through a planar curve normal to a curve tangent to a surface from its equation mean through points
q
q
q
q
q
q
q
q
q
Open the Planes1.
A plane is displayed offset from the reference plane. it is represented by a red square symbol.

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Use the Reverse Direction button to reverse the change the offset direction.FreeStyle Shaper. each separated from the initial plane by a multiple of the Offset value. or simply click on the arrow in the geometry.
As many planes as indicated in the dialog box are created (including the one you were currently creating).
.
Parallel through point
q
Select a reference Plane and a Point.
q
Click the Repeat object after OK if you wish to create more offset planes . the Object Repetition dialog box is displayed. and you key in the number of instances to be created before pressing OK. In this case.

To select the latter press and hold the Shift key while moving the pointer over the element. then click it. This axis can be any line or an implicit element. such as a cylinder axis for example.
Angle or normal to plane
q
Select a reference Plane and a Rotation axis. Profiler & Optimizer
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A plane is displayed parallel to the reference plane and passing through the selected point.
q
. Enter an Angle value.FreeStyle Shaper.

FreeStyle Shaper. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry. each separated from the initial plane by a multiple of the Angle value.
This plane type enables to edit the plane's parameters. As many planes as indicated in the dialog box are created (including the one you were currently creating).
. Here we created five planes at an angle of 20 degrees. In this case. and you key in the number of instances to be created before pressing OK.
Through three points
q
Select three points. Profiler & Optimizer
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A plane is displayed passing through the rotation axis. the Object Repetition dialog box is displayed. It is oriented at the specified angle to the reference plane.
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Click the Repeat object after OK if you wish to create more planes at an angle from the initial plane.

The plane passing through the two line directions is displayed. When these two lines are not coplanar. Profiler & Optimizer
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The plane passing through the three points is displayed. the vector of the second line is moved to the first line location to define the plane's second direction.FreeStyle Shaper.
Through two lines
q
Select two lines.
. You can move it simply by dragging it to the desired location.

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Check the Forbid non coplanar lines button to specify that both lines be in the same plane.
Through point and line
q
Select a Point and a Line.
The plane passing through the point and the line is displayed.
.FreeStyle Shaper.

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A plane is displayed tangent to the surface at the specified point.
Normal to curve
q
Select a reference Curve.FreeStyle Shaper.
q
. By default. the curve's middle point is selecte. You can select a Point.

FreeStyle Shaper.
q
.
Mean through points
q
Select three or more points to display the mean plane through these points.
It is possible to edit the plane by first selecting a point in the dialog box list then choosing an option to either:
q
Remove the selected point Replace the selected point by another point. Profiler & Optimizer
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A plane is displayed normal to the curve at the specified point.

B. C. D components of the Ax + By + Cz = D plane equation. you are able to modify A. B. the D component becomes grayed.
Select a point to position the plane through this point. Profiler & Optimizer
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Equation
q
Enter the A.
Use the Normal to compass button to position the plane perpendicular to the compass direction.FreeStyle Shaper. Use the Parallel to screen button to parallel to the screen current view.
. and C components.

For more information. Profiler & Optimizer
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3.FreeStyle Shaper. You can isolate a plane in order to cut the links it has with the geometry used to create it.
q
Parameters can be edited in the 3D geometry. use the Isolate contextual menu. To do so. refer to the Editing Parameters chapter. Click OK to create the plane.
q
. The plane (identified as Plane. refer to the Isolating Features chapter. For more information.xxx) is added to the specification tree.

Please note that you need to put the desired geometrical set in show to be able to perform the corresponding scenario. the corresponding circle or circular arc is displayed.
Center and radius
q
Select a point as circle Center. Start and End angles can be specified by entering values or by using the graphic manipulators.
If a support surface is selected.
. Enter a Radius value. Profiler & Optimizer
Creating Circles
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This task shows the various methods for creating circles and circular arcs:
q
center and radius center and point two points and radius three points center and axis bitangent and radius bitangent and point tritangent center and tangent
q
q
q
q
q
q
q
q
Open the Circles1. you can specify the Start and End angles of the arc. For a circular arc. Click the Circle icon . 2. Use the drop-down list to choose the desired circle type. 1.FreeStyle Shaper.CATPart document. Select the Support plane or surface where the circle is to be created.
q
q
Depending on the active Circle Limitations icon. the circle lies on the plane tangent to the surface at the selected point.
The Circle Definition dialog box appears.

to display the alternative arc. you can specify the trimmed or complementary arc using the two selected points as end points. which center is the first selected point and passing through the second point or the projection of this second point on the plane tangent to the surface at the first point. is previewed. Depending on the active Circle Limitations icon.
q
q
The circle.
q
q
The circle. Select the Support plane or surface where the circle is to be created. is previewed. you can specify the Start and End angles of the arc.
Two points and radius
q
Select two points on a surface or in the same plane. For a circular arc. Enter a Radius value. passing through the first selected point and the second point or the projection of this second point on the plane tangent to the surface at the first point. the corresponding circle or circular arc is displayed. Select a Point where the circle is to be created.FreeStyle Shaper. You can use the Second Solution button. For a circular arc. Depending on the active Circle Limitations icon.
. Profiler & Optimizer
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Center and point
q
Select a point as Circle center. Select the Support plane or surface. the corresponding circle or circular arc is displayed.

Set the Project point on axis/line option: r checked (with projection): the circle is centered on the reference point and projected onto the input axis/line and lies in the plane normal to the axis/line passing through the reference point. Select a point.
Depending on the active Circle Limitations icon. you can specify the trimmed or complementary arc using the two of the selected points as end points.
Center and axis
q
Select the axis/line. It can be any linear curve.
r
q
q
q
unchecked (without projection): the circle is centered on the reference point and lies in the plane normal to the axis/line passing though the reference point. For a circular arc. Enter a Radius value.FreeStyle Shaper.
With projection
Without projection
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Three points
q
Select three points where the circle is to be created. The line will be extended to get the projection if required. the corresponding circle or circular arc is displayed.

If an explicit Support needs to be defined. Select a Support surface. so click in the region where you want the circle to be. For a circular arc. a contextual menu is available to clear the selection in order to select the desired support.
These options are only available with the Trimmed Circle limitation.
q
If one of the selected inputs is a planar curve. This automatic support definition saves you from performing useless selections. then the Support is set to Default (Plane).
You can select the Trim Element 1 and Trim Element 2 check boxes to trim the first element or the second element. or both elements.
. you can specify the trimmed or complementary arc using the two tangent points as end points.
q
Enter a Radius value. Several solutions may be possible. the corresponding circle or circular arc is displayed.
q
Depending on the active Circle Limitations icon. Here is an example with Element 1 trimmed. Profiler & Optimizer
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Bi-tangent and radius
q
Select two Elements (point or curve) to which the circle is to be tangent.FreeStyle Shaper.

If one of the selected inputs is a planar curve. the corresponding circle or circular arc is displayed.
Depending on the active Circle Limitations icon. you can choose the trimmed or complementary arc using the two tangent points as end points.
q
q
The point will be projected onto the curve. Select a Support plane or planar surface.
q
Several solutions may be possible.
Complementary trimmed circle
. or both elements.
Complete circle For a circular arc. If an explicit Support needs to be defined. Select a Curve and a Point on this curve. These options are only available with the Trimmed Circle limitation.FreeStyle Shaper.
Trimmed circle You can select the Trim Element 1 and Trim Element 2 check boxes to trim the first element or the second element. Profiler & Optimizer
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Bi-tangent and point
q
Select a point or a curve to which the circle is to be tangent. Here is an example with both elements trimmed. so click in the region where you want the circle to be. then the Support is set to Default (Plane). This automatic support definition saves you from performing useless selections. a contextual menu is available to clear the selection in order to select the desired support.

FreeStyle Shaper. For a circular arc. the corresponding circle or circular arc is displayed. The first and third elements define where the relimitation ends. Select a Support planar surface.
Center and tangent
There are two ways to create a center and tangent circle:
. If an explicit Support needs to be defined. then the Support is set to Default (Plane). This automatic support definition saves you from performing useless selections. so select the arc of circle that you wish to create. a contextual menu is available to clear the selection in order to select the desired support.
These options are only available with the Trimmed Circle limitation.
Depending on the active Circle Limitations icon.
q
Several solutions may be possible. you can specify the trimmed or complementary arc using the two tangent points as end points.
q
If one of the selected inputs is a planar curve.
You can select the Trim Element 1 and Trim Element 3 check boxes to trim the first element or the third element. Profiler & Optimizer
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Tritangent
q
Select three Elements to which the circle is to be tangent. or both elements. Here is an example with Element 3 trimmed.

Select a Tangent Curve. the axes are not aggregated under the Circle features.
q
4. The circle (identified as Circle. If the datum mode is active. Center curve and radius
q
Select a curve as the Center Element. an axis normal to the circle will be created. If you select a direction.xxx) is added to the specification tree.FreeStyle Shaper.
q
You can click the Diameter button to switch to a Diameter value. This option is available with the Center and radius.
r
If you do not select a direction. Center and tangent.
q
You can select the Axis computation check box to automatically create axes while creating or modifying a circle. and Center and axis circle types.
q
The circle center will be located either on the center curve or point and will be tangent to tangent curve. Conversely. This automatic support definition saves you from performing useless selections.
r
In the specification tree. Line tangent to curve definition
q
Select a point as the Center Element. but one ore three datum lines are created. Bi-tangent and radius. If an explicit Support needs to be defined.
.
q
q
2.
q
q
If one of the selected inputs is a planar curve. the Axis direction field is enabled. Enter a Radius value. Select a Tangent Curve. You can edit their directions but cannot modify them. click the Radius button to switch back to the Radius value. Two point and radius. Click OK to create the circle or circular arc. Note that the value does not change when switching from Radius to Diameter and vice-versa. Once the option is checked. then the Support is set to Default (Plane). Profiler & Optimizer
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1. a contextual menu is available to clear the selection in order to select the desired support. the axes are aggregated under the Circle feature. two more axes features will be created: an axis aligned with the reference direction and an axis normal to the reference direction. Please note that only full circles can be created.

use the Isolate contextual menu. then the Axis Computation is not possible. You can isolate a plane in order to cut the links it has with the geometry used to create it. Parameters can be edited in the 3D geometry. click the Next Solution button to move to another arc of circle.
q
q
.FreeStyle Shaper. or directly select the arc you want in the 3D geometry. To do so. refer to the Editing Parameters chapter. refer to the Isolating Features chapter. This option is available with the Center and radius. Two point and radius. In this case just select a support surface. Profiler & Optimizer
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Axis aligned with the reference Axis normal to the reference direction Axis normal to the circle direction (yz plane) (yz plane) If you select the Geometry on Support option and the selected support is not planar. When several solutions are possible. For more information. You can select the Geometry on Support check box if you want the circle to be projected onto a support surface. Center and point. For more information. and Three points circle types.
q
q
A circle may have several points as center if the selected element is made of various circle arcs with different centers.

All FreeStyle commands are thus available at all times in this mode.Publications Exposed) and Explode (Document not kept). when saving data into ENOVIA V5. To ensure seamless integration.
. Therefore. you must have both a CATIA and ENOVIA session running. ENOVIA V5 offers two different storage modes: Workpackage (Document kept . Profiler & Optimizer
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Optimal CATIA PLM Usability for FreeStyle
When working with ENOVIA V5. some CATIA V5 commands are grayed out / hidden in the FreeStyle workbench. In FreeStyle workbench. the global transaction is guaranteed but only if the target is in Workpackage mode. in interoperability mode. the safe save mode ensures that you only create data in CATIA that can be correctly saved in ENOVIA.FreeStyle Shaper.

or whether they are currently selected or not See Scanning a Part and Defining In Work Objects
Hide
In Work Object
Analysing Using Parameterization Analysis.. Allows editing parameters and formula Allows capturing images Allows recording...... It also allows you to define visualization options. Please note that most of the Tools commands available here are common facilities offered with the Infrastructure. Standards. and manage the compass specifically for the FreeStyle Shaper.. Allows layer filters management Allows customizing settings Managing Standards in the Interactive Drafting documentation Allows setting up of communication tools
Visualization Options
For. For. Profiler & Optimizer
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The Tools menu lets you perform image capture and album management... Options. Optimizer and Profiler elements. Specific Generative Shape Design commands are described in the present document. Conferencing Visualization Options Compass Orientation View Manipulation Allows customizing the workbench... Show See.. See. running and editing macros Using the Batch Monitor Allows to show a set of elements according to their type. set user preferences and manage macros... Visualization Filters. Parameterization Visualisation Options Compass Orientation View Manipulation Customize.. Formula Image Macro Utility. or whether they are currently selected or not Allows to hide a set of elements according to their type... Apply DressUp Setting Visualization Options
.FreeStyle Shaper.. Refer to the Infrastructure User's Guide... viewpoints.

and the product in general.
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Help
The Help menu lets you get help on the currently active command. Refer to the Infrastructure User's Guide.

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Creation Toolbars
The creation toolbars contain the following tools:
See Creating Planar Patches See Creating a Surface from Three Points See Creating a Surface from Four Points See Creating a Surface on a Existing Surface See Extruding a Surface See Creating Revolution Surfaces See Offsetting a Surface See Extrapolating Curves See Creating Blend Surfaces See Creating an ACA Fillet See Creating Filling Surfaces See Creating Associative Filling Surfaces See Creating a Net Surface (Freestyle Profiler) See Creating Swept Surfaces (Freestyle Profiler)
.

Smoothing Curves.FreeStyle Shaper. Editing Surfaces Using Control Points and Smoothing Surfaces See Matching Surfaces See Multi-side Matching See Fitting a Curve to a Cloud of Points and Fitting a Surface to a Cloud of Points (Freestyle Optimizer) See Globally Deforming Surfaces (Freestyle Optimizer) See Extending a Curve and Extrapolating a Surface
See Redefining Surface Limits See Restoring a Surface See Fragmenting Curves and Fragmenting Surfaces See Concatenating Curves See Disassembling Elements See Approximating/Segmenting Curves or Approximating/Segmenting Surfaces See Copying Geometric Parameters
. Profiler & Optimizer
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Modification Toolbars
The modification toolbar contains the following tools:
See Performing a Symmetry on Geometry See Editing Curves Using Control Points.

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Analysis Toolbar
The analysis toolbar contains the following tools:
See Checking Connections Between Elements See Checking Connections Between Curves See Analyzing Distance Between Two Sets of Elements See Performing a Curvature Analysis See Using Dynamic Cutting Planes See Analyzing Reflect Curves (Freestyle Optimizer) See Creating Inflection Lines (Freestyle Optimizer) See Analyzing Using Highlight Lines See Performing a Surfacic Curvature Analysis See Performing a Draft Analysis See Mapping an Environment on a Surface See Analyzing Using Isophotes See Analyzing Using Highlights See Manipulating Light Sources
.

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Generic Tools Toolbar
The generic tools toolbar contains the following tools:
See Setting FreeStyle Visualization Options See Setting FreeStyle Visualization Options See Displaying a Part Symmetrically See Displaying Geometric Information on Elements See Managing the Compass See Defining an Axis System See Working with a 3D Support
.

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FreeStyle Dashboard
The FreeStyle Dashboard contains the following tools:
See Creating Datums See Keeping the Initial Element See Inserting in a New Geometrical Set See Creating a Temporary Analysis See Auto detection
See Attenuation
See Displaying Manipulators on Elements
See Displaying Control Points Temporarily
.FreeStyle Shaper.

Click the Shape category in the left-hand box. Click OK when done. Set options in these tabs according to your needs. 1. display and tuning options. 3.
4.FreeStyle Shaper. auto detection. you can customize the way you work to suit your habits. 5. This type of customization deals with permanent setting customization: these settings will not be lost if you end your session.
2. Click the FreeStyle workbench The General tab is displayed. Select the Tools -> Options menu item. Profiler & Optimizer
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Customizing
Before you start your first working session.
.
The General tab lets you define geometry. The Options dialog box appears.

the Max order is set to 16 and cannot be modified. In P1 mode.
Order
This option lets you set the maximum allowed order along the U (and V) directions for each curve segment and surface patch.FreeStyle Shaper. Optimizer. In this case you accept the conversion up to the set tolerance value. the constraint tolerance value is set and cannot be modified. and Profiler
This page deals with the following options:
q
Geometry Auto detection Display Tuning
q
q
q
Geometry
Tolerances
This option lets you impose user-defined tolerances to every element to be created and modified within a FreeStyle workbench. Profiler & Optimizer
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FreeStyle Shaper. You can define: q the constraint tolerance value used to define the continuity variation.
q
the deviation tolerance value. This maximum order value ranges from 5 to 16 included.
. In P1 mode. Optimizer. used when converting elements using the Converter Wizard for example (see tasks "Approximating/Segmenting Procedural Curves" and "Approximating/Segmenting Procedural Surfaces" within the FreeStyle Shaper. and Profiler User's Guide). in a given direction. In this case if the continuity is over the set value the element is not created/modified.

By default. this option is unchecked. this option is checked. See "Displaying Control Points Temporarily" in the FreeStyle Shaper.
Continuity
.
Display
This area lets you set the information to be displayed on the geometry as you manipulate it. This option allows the display of control points on geometry detected with the pointer when using the Snap on Cpt (snap on control points) option from the Dashboard. and Profiler User's Guide).
Search Dressing
You can choose to display the dressing mode by selecting the Search dressing checkbox. Optimizer. Profiler & Optimizer
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Auto Detection
Coordinates
You can choose to display the point coordinates as the pointer moves along the geometry by selecting the Coordinates checkbox By default.
Control Points
Displays the Control Points on the geometry.FreeStyle Shaper.

and so forth)
. and so forth)
Order
Displays the Order number along the U (for curves) or U and V directions (for surfaces).FreeStyle Shaper.
Contact Point
Displays the Contact Point at every connection between connected elements (such as blend and match curves and surfaces. and so forth)
Curvature
Displays the Curvature texts on an element (such as blend and match curves and surfaces. Profiler & Optimizer
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Displays the Continuity at every connection between elements (such as blend and match curves and surfaces. fill surfaces.

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Tension
Displays the Tension manipulators at every connection between connecting elements (such as blend and match curves and surfaces.FreeStyle Shaper. and so forth)
By default. and "Manipulating Views" in the FreeStyle Shaper. neither of the above options is selected. Optimizer.
. and Profiler User's Guide for example. See "Editing Surfaces Using Control Points".
Tuning
This area lets you set the values used when manipulating views or geometry (P2 only).

e. It is displayed whenever you are creating an element or applying modifications to this element. The 3D compass is a three-axis system used to define the plane into which any action is performed. for example the curvature of the surface.
blend curve
blend surface A surface created to connect two pre-existing surfaces
C
chain of curves cloud of points A chain of curves contains at least one curve. This error is an absolute error. and it is measured in mm or inches. If one edge of surface S1 meets an edge of the surface S2 then we say along this edge both surfaces are connected with the order of continuity G0. Fillet. If there are more than one curve. A 2-D Curve does not follow the modification of the surface. A 3D-Curve placed on a surface does not yield any information about the surface.
B
basic surface If a surface is trimmed at an arbitrary curve. A cloud of points may consist of a single point or several million points. Normally a curve is a 3D-Curve. A face has an underlying Basic Surface. A curve created to connect two pre-existing curves. If the G0-continuity is missed then we have a so called G0-error. Profiler & Optimizer
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Glossary
Special Characters
2D-Curve A 2D-Curve is defined in the u-v-Parameterspace of the surface. Gaps and overlapping are not allowed. A set of points in space. the endpoint of the first curve has to meet the start point of the second curve and so on. A 2D-Curve yields information of the surface.
F
face feature modeling A face is a trimmed surface.
G
G0 If the endpoint of curve K1 meets the endpoint of curve K2 then we say: At this point both curves are connected with order of continuity G0.g. Some Commands. This input surface is called Basic Surface (if it is not trimmed).
. If you modify the surface there will be a gap between the 2-D Curve and the surface.
3D compass
3D-Curve
A
approximation A surface or a curve is converted into a NUPBS surface or a NUPBS curve. A trimmed surface is called a face and the underlying untrimmed surface is called the Basic surface. a distance. have the Option Feature Modeling. The term Feature Modeling is explained with the Command ACA Fillet. it is sometimes wanted that the trimmed surface yields the information about the input surface.FreeStyle Shaper. attenuation Factor to attenuate the speed with of the mouse displacement.

The Gaussian curvature is calculated from the Max Principal and the Min Principal curvature with the following formula: Gauss = sig(MaxPrincCurvature)*sig(MinPrincCurvature)*sqrt(abs(MaxPrincCurvature*MinPrincCurvature)) Sig is the sign (of MaxPrincCurvature and MinPrincCurvature) and can only have the value +1 or 1. If both curves in the point P run into the same direction. and it is measured in deg of rad and it is the G1-error of the envelope. For the definition of the G3-continuity we look at the curvature hedgehog. This error is a relative error and it is calculated with the following formula. This error is an absolute error. Sometimes this error is measured in percent % then its maximum is 200%. and it is measured in deg of rad. If the normal does not change its angle from one point of the border of S1 to the nearest point of S2 then we say the order of continuity is G1. and types of deformation. then we say the order of continuity is G2. We take the normal of S1 in a point near the curve C and run with this normal over the border to S2. while taking the continuity type into account. We look at the curvature vector of K1 in point P and the curvature vector of K2 in point P. match surface A surface deformed so as to connect another surface. then we have a so called G3-error between both curves. If both vectors have the same direction and the same absolute value. This error is an absolute error. an angle. The curve K1 and the curve K2 are connected with the order of continuity G1 in the point P. The surface S1 and the surface S2 are connected with the order of continuity G0 along the curve C. which curvature value is 0 at each point. an angle.
. K1 may have the radius R and K2 may have the radius r at the common point. mesh line A line on a surface used to deform this surface according to various laws. as it can be created with the command Porcupine Curvature Analysis.
I
inflection line Curve. If the G3-continuity between both curves is missed. If this envelope has at the desired point G1-continuity then we say the order of continuity between both curves is G3. while taking the continuity type into account. isophote A line or surface on a chart forming the locus of points of equal illumination or light intensity from a given source. then we say the order of continuity is G1. If each curve on S1 which runs over the border to S2 can be continued with another curve on S2 and their order of continuity is G2 then we say both surfaces are connected with the order of continuity G2. with r<R. as opposed to a deformation successively applied to different elements.FreeStyle Shaper. Profiler & Optimizer
G1
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The curve K1 and the curve K2 are connected with the order of continuity G0 in the point P.
G2
G3
The curve K1 and the curve K2 are connected with the order of continuity G2 in the point P. G3-continuity between surfaces is defined on the curves between both surfaces on the same way. If the G1-continuity is missed then we have a so called G1-error. We look at the envelope of the curvature hedgehog. then yields: error= 2*(R-r)/(R+r) The maximum of this error is 2.
Gaussian curvature
global deformation
A deformation that is applied globally to a set of elements. lying on a surface. the G1-continuity of the envelope is missed. this means the angle between the tangents of both curves is 0. If the G2-continuity is missed then we have a so called G2-error. The surface S1 and the surface S2 are connected with the order of continuity G1 along the curve K.
M
match curve A curve deformed so as to connect another curve.

Non Uniform B-Spline is also called NUPBS. See Surface. A surface can be trimmed for example by the command Break. A surface has an order in u.FreeStyle Shaper. See NURBS.and an order in v-Direction. is a NUBS with a rational component. Profiler & Optimizer
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N
NUPBS NURBS A NUBS. With a Rational Curve a Circle and a Hyperbola can be described exact. A trimmed surface is called Face and contains all the information of the untrimmed surface. An operation retaining the topological properties of the element undergoing the specified transformation.
. The command Geometric Information shows you in the panel Geometric Analysis the available information. that reflects the light emanating from a grid of neon located above the surface.
S
surface In CATIA. The simplest surface is a 4-Point-Patch of order 2 in u-Direction and order 2 in v-Direction. A surface can have only one patch or several patches. 2<=order<=16.
U
untrimmed surface See Surface. A NURBS.
R
reflection line A curve visualized on a surface. Non Uniform Rational B-Spline. It can be untrimmed by the command Untrim. surfaces are parameterized with the u. Because of this a command can work on the Face or on the (untrimmed) Basic Surface.
T
topological topological operation trimmed surface Concerned with relations between objects abstracted from exact quantitative measurements. Rational means that the weight of the Control Points must not have the value 1.and v-Parameters running from 0 to 1. to make it more clear that it is a polynomial curve and not a rational curve.